Like the title says, this isn't about ONE and TWO.  This is about the little things.  Small, minor bugs that make you wish SOLIDWORKS was a person so that you could build a time machine to go back and murder its parents.  Bonus points if the problem is just intermittent enough to make you forget about it, until it happens again.

 

Be sure to post your SOLIDWORKS version and service pack, just in case someone wants to verify your bug or let you know that it is fixed in later versions.  I'll give one for starters.

 

SW2016 SP 2.0

  • Often, but not always, when typing in the property manager (renaming features, entering dimension text, etc) the hotkey for the letter I type will activate.  I suspect it has to do with typing speed.  It has done this for as long as I can remember.

Categories: General

Comments
Last comment By: Jim Wilkinson   Wed, 07 Mar 2018 12:00:54 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Alex Lachance wrote:

 

Hey Dennis,

 

I work with flexibles a bit. Few things I noticed:

 

First off : I've noticed that flexible assemblies tend to lose their flexibility when you restart SolidWorks. Often, a simple toggle of ''Rigid'' back to ''flexible'' fixes it.

 

Second : It might seem like a stupid question but is your flexible assembly built around your assembly's environment? It is an error I often see here, people trying to build flexible assemblies without mating their part to the assembly's environment. What I call the environement is the things that cannot move. Origins, Planes, axes if you've set your template to have axes, stuff like that.

 

Third : Is your flexible assembly's environment minimally mated with your top level assembly's environment? That is another mistake I often see. You don't need to set all 3 planes to coincident, but at least one. If you don't do this, then you need to make sure the component that is used to ''fix'' your flexible assembly is indeed ''fixed'' in the flexible assembly.

 

Last : When you unroll the tab, is there some - left next to some parts?

 

 

 

Flexible's aren't the most reliable though so I try to use them as least as possible. The times I use them is when it truely requires to be installed ''on site'', or when I need to do a study of movement.

 

I'm on 2016 too so maybe 2017 has had some tweaks that make it a little more buggy..?

 

Edit: It is imperative that you do not use the ''lock rotation'' when using flexible assemblies too. Use a parralel mate to lock the rotation. As stated by Jim, these often cause errorrs. It is kind of linked to one I posted last week about concentric lock not being able to rotate on itself

Mates have been a challenge for as long as I can remember using SW and over the years I have tried to find ways to trick SW so the mates are stable.  The mates that create issues when going from Rigid to Flexible are most often.. Tangent, Limited Distance and Cam mates, so if you use other methods such as using sketch lines or splines the assemblies will remain stable and perform much better.

I am really hoping that SPR #1051495 will get implemented in the near future, because it will revolutionize the mate process and would basically make the (3) three mentioned mates obsolete. 

Another thing is that most people talk about having (3) mates to lock in the parts, however in most cases you can use (2) two mates and the components are fixed, this is achieved be just adding a L shaped sketch or the mate selections are L shaped per the samples below... (anytime you can reduce mates the better the performance, 100 parts - 3 mates = 300 individual mates, if you can cut 1 mate per part that's 100 less mates) 

 

 

For circular items you just need to add a simple L shaped sketch to achieve the same results, such as the plate and screw below

 

 

 

By: John Stoltzfus  Wed, 06 Dec 2017 12:05:43 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Mates have been a challenge for as long as I can remember using SW and over the years I have tried to find ways to trick SW so the mates are stable.  The mates that create issues when going from Rigid to Flexible are most often.. Tangent, Limited Distance and Cam mates, so if you use other methods such as using sketch lines or splines the assemblies will remain stable and perform much better.

I am really hoping that SPR #1051495 will get implemented in the near future, because it will revolutionize the mate process and would basically make the (3) three mentioned mates obsolete.

Another thing is that most people talk about having (3) mates to lock in the parts, however in most cases you can use (2) two mates and the components are fixed, this is achieved be just adding a L shaped sketch or the mate selections are L shaped per the samples below... (anytime you can reduce mates the better the performance, 100 parts - 3 mates = 300 individual mates, if you can cut 1 mate per part that's 100 less mates)

 

For circular items you just need to add a simple L shaped sketch to achieve the same results, such as the plate and screw below

That's a pretty neat trick, though I hate having sketches showing everywhere. How do you work with this method so that the sketches don't annoy you? Do you have a hotkey to switch from Sketches shown to sketches hidden?

By: Alex Lachance  Wed, 06 Dec 2017 12:56:11 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

You misunderstood my post.  In my case, the problem with flexibility was solved bylocking the rotation of a concentric mate of a part.

 

I understood your post but as you pointed out there are many inconsistencies in flexible assemblies. I was merely pointing out that the lock rotation is one that causes me alot of headaches. Sorry if I might have put words in your mouth by mistake.

 

I have some flexible assemblies which are just too flexible and SolidWorks doesn't like it. This is one of them. It is a trailer landing gear. The landing gear is flexible in terms of frame width. It's footing is also flexible as it can move from the closed position to the open position(still from flexibile). There are 6 braces on the assembly, they are all flexible with a limit distance mate.

 

 

SolidWorks hates it and so do I, it's just too flexible.

By: Alex Lachance  Wed, 06 Dec 2017 12:50:16 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

They way I would handle it is hide and show the sketches as needed, with the parts I'm working on, nothing automatic.  The time it takes to hide or show the sketches is offset by having a stable assembly.  I would much rather do that then deal with what you're showing above...

By: John Stoltzfus  Wed, 06 Dec 2017 13:02:03 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

How's bout, having to close and re-open solidworks numerous times daily because it doesn't dump the memory?

 

This may have been addressed in future releases, were still running 2014.

 

On a normal day, I get numerous requests where I have to go in and open many many different parts, assemblies and drawings in a short period of time.

By the time I'm done opening and closing all the files, and am back to the part drawing im working on, my resources are pegged.

By: Anthony Macke  Wed, 06 Dec 2017 16:23:39 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

also, angle dimensions on drawings. why can i click 4 miles away from anything, in the middle of nowhere, and move an angle dimension?

By: Anthony Macke  Wed, 06 Dec 2017 16:24:40 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Anthony    wrote:

 

How's bout, having to close and re-open solidworks numerous times daily because it doesn't dump the memory?

 

This may have been addressed in future releases, were still running 2014.

 

On a normal day, I get numerous requests where I have to go in and open many many different parts, assemblies and drawings in a short period of time.

By the time I'm done opening and closing all the files, and am back to the part drawing im working on, my resources are pegged.

Check this out:

 

SOLIDWORKS low resources – What’s holding my RAM hostage? | Computer Aided Technology

By: Dan Pihlaja  Wed, 06 Dec 2017 16:44:16 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Daen Hendrickson wrote:

 

I am using SW2014 SP5.

 

When I have a drawing view that has been rotated to a non-90° increment hole center marks are not centered. For hole series I use a linear center mark. The initial center mark is aligned with horizontal/Vertical of the view and then the second center mark defines the alignment angle. My intuition is that the amount the center marks are not centered is related to the amount they must be rotated.

 

View rotated a few degrees so that the top edge is horizontal with the sheet. First center mark aligned with view's un-rotated horizontal/vertical. Center point is still NOT aligned with hole. (Although a slot is shown, I see the same behavior with holes). This is a sheet metal part.

 

After the second center mark is added and the linear connection line is generated...

 

This behavior has been there for as long as I can recall. I have not found a good work-around. Manually sketching center marks is one approach but NOT preferred. I usually just "grin and bear it".

 

Daen

One work around is to use "Relative to Model" instead of rotating the view.

By: Dan Pihlaja  Wed, 06 Dec 2017 18:11:17 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I am using SW2014 SP5.

 

When I have a drawing view that has been rotated to a non-90° increment hole center marks are not centered. For hole series I use a linear center mark. The initial center mark is aligned with horizontal/Vertical of the view and then the second center mark defines the alignment angle. My intuition is that the amount the center marks are not centered is related to the amount they must be rotated.

 

View rotated a few degrees so that the top edge is horizontal with the sheet. First center mark aligned with view's un-rotated horizontal/vertical. Center point is still NOT aligned with hole. (Although a slot is shown, I see the same behavior with holes). This is a sheet metal part.

 

After the second center mark is added and the linear connection line is generated...

 

This behavior has been there for as long as I can recall. I have not found a good work-around. Manually sketching center marks is one approach but NOT preferred. I usually just "grin and bear it".

 

Daen

 

EDIT: Knowledge base lists SPR: 900250 which says this is a result when Options>Document Properties>Detailing>Center of Mass> Scale by view scale is unchecked... which mine is. However, checking the box did not correct the existing center marks. Deleting and recreating also did not correct the center marks.

By: Daen Hendrickson  Wed, 06 Dec 2017 18:03:28 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Dan Pihlaja wrote:

 

One work around is to use "Relative to Model" instead of rotating the view.

Dan,

 

That does correct the center mark issue. But it won't allow me to show bend notes of a flat pattern - the option under drawing view properties is grayed out. The offset center mark is the lesser of two evils in my case.

 

Good fix regardless. I often forget about the relative view.

 

Daen

By: Daen Hendrickson  Wed, 06 Dec 2017 18:19:13 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

A great resource Dan Pihlaja! Thank you!!

By: Edward Poole  Wed, 06 Dec 2017 18:21:19 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Daen Hendrickson wrote:

 

Dan Pihlaja wrote:

 

One work around is to use "Relative to Model" instead of rotating the view.

Dan,

 

That does correct the center mark issue. But it won't allow me to show bend notes of a flat pattern - the option under drawing view properties is grayed out. The offset center mark is the lesser of two evils in my case.

 

Good fix regardless. I often forget about the relative view.

 

Daen

I wasn't aware of that limitation.  Good to know.  Thanks!

By: Dan Pihlaja  Wed, 06 Dec 2017 18:38:54 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

View scale, why does it have be a click fest every time you want to put in a "User Defined" scale? Why even have "User Defined" locked away like that. Why not just click on the view and put any scale you want? Instead of

 

Click "Use Custom Scale"

Click "Down Arrow"

Scroll

Click "User Defined"

Click Change the Scale.

 

Really in 2017....?

 

SolidWorks must be the most click heavy CAD package. With arthritic fingers, it gets to be a literal pain some days.

By: Greg Young  Wed, 06 Dec 2017 20:19:56 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

The scales are default scales offered, Some people would rather click on the ''down arrow'' and then select 1:4 then click and have to type 1:4.

 

The reason it is built that way is because of the possibilities of your scale being linked to something else.

 

Perhaps they could add a 4rth icon that is the ''User defined custom scale'' which would give you exactly what you want while leaving what is already there as it is for those users that like it that way.

By: Alex Lachance  Wed, 06 Dec 2017 20:24:35 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

There are way around that - I don't hardly ever change my scale that way, don't touch it.  I have macro buttons

 

Select the drawing view and select the macro button and that's it...

 

There are a lot of ways around what SW thinks you should do...

By: John Stoltzfus  Wed, 06 Dec 2017 20:37:23 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I have colleagues that use the quick mates a lot. One thing that annoys them is the inability to reverse the direction of the mate upon agreeing to it.

 

I tried searching through the KB but found nothing.

By: Alex Lachance  Wed, 06 Dec 2017 20:42:26 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I'm one of those that gets EXTREMELY annoyed when I click and a bunch of mates fail and I have to go back and delete the mate I just put in and do it all over again - Such a pain. Fortunately I have gotten good at keeping my frustration voice as a workplace voice and not an outside voice.

By: Rick McDonald  Wed, 06 Dec 2017 21:55:10 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Rick McDonald wrote:

 

I'm one of those that gets EXTREMELY annoyed when I click and a bunch of mates fail and I have to go back and delete the mate I just put in and do it all over again - Such a pain. Fortunately I have gotten good at keeping my frustration voice as a workplace voice and not an outside voice.

It is strange, isn't it? You create exactly the same mate and it works second time round.

By: Wayman John  Thu, 07 Dec 2017 08:56:35 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

The one I like with mating is it always seems like the first mate fails. If I want to add a distance mate, it will default to a coincident mate which always seems to work but when you then change that mate to a distance mate while still in the mating command, it inevitably fails. Why if the coincident mate was going to work, would the distance mate fail, especially if it is the 1st mate added to a part.

By: John Lhuillier  Thu, 07 Dec 2017 12:31:50 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

All bugs that have been mentioned + another 1000 that i experiance in 2018 sw. It is very bug-friendly version.

One that drives my crazy is that bendlines of sheet parts in main assemblies  keep coming back even when they are hiddend everywhere. They just always come back when I re-open my assemlies. Or atleast some of them. Gosh that gives me headache!!!! Even now just by talking about it!!!!

By: Fred Vraj  Thu, 07 Dec 2017 12:34:29 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Originally posted here: When using quotes (double prime) for inch math operation does not work

 

With regards to the Double Prime mark for inch units: "

It works in the dimension modification box as long as you don't create an equation out of it.

 

So these all work:

 

But this doesn't work:

 

 

As soon as an equation is introduced, the double prime no longer works.

By: Dan Pihlaja  Thu, 07 Dec 2017 15:27:23 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I'm not quite sure this qualifies as a bug. Why is it possible to do an ''unfold'' function for sheet metal without having any bends selected?

 

This doesn't give any error:

By: Alex Lachance  Thu, 07 Dec 2017 16:16:24 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

This is not really a bug, but more of an annoying inconsistency between solidworks and most text editing programs on windows. Say I want to change the font of a note to arial 12 pt. In word I can select the text, place the cursor in the font search box, type arial, hit tab, type 12, done. One mouse move, the rest is keyboard.  

 

In solidworks this is not as fluid.  Many more precise mouse clicks and transitions between keyboard and mouse are required because it is not possible to tab between the different fields in the formatting toolbar. Also, the only way to select a font is to click on it, even if you enter it exactly in the search box.

 

Every time I copy and paste notes from other programs into solidworks I have to do this operation. If you could make the functionality of your font selection mimic the flow of word's it would make for a better experience.

 

Captured.JPG

 

Capture.JPG

By: Colt Carson  Thu, 07 Dec 2017 19:57:39 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

One that really gets me is the mirror components feature. Working with sheetmetal parts in an assembly it's super handy to use mirror to create the opposite hand parts. But, when you try to add a handed part to the mirror feature it decides to recreate all of the already created mirrored parts assigning them new part numbers at the same time...

By: Michael Van Dorp  Fri, 08 Dec 2017 18:13:50 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Michael,

If you would add this to the top 10 list I would definitely add my vote to this. We should have the opportunity to select which parts to create and which ones to not create.

By: Jim Steinmeyer  Fri, 08 Dec 2017 20:17:34 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Stupid *bug* of the day:

 

I had an assembly where someone didn't put clinch nuts on the brackets i.e. just a bit of sheet, not an assy. Swine!

 

I made an assy, added the clinch nuts, and replaced the part in the assy - no problems reported, click ok. Then, Error!! Mating problems!! Spent ages trying to figure out the guilty culprit.

 

Suppress the assy and then unsuppress... error gone...? I did this quite a few times. Consistently non-existent error.

By: Martin Tofts  Mon, 11 Dec 2017 15:39:11 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I just spent some considerable time making a Pack & Go copy of an assembly. I needed to make new copies of less than half of the parts and re-use the remainder, so I clicked the top box to un-select all the parts first. I then typed in all the new names for the copied parts and their drawings, set the directory and clicked Save.

When I opened the new assembly, it was still using all of the old parts, because, when you type a new name in the Save To Name column of Pack & Go, it does not check the box to include that part in the Pack & Go! You then have to go back and individually check the include box for every new part and drawing.

I realise that I really should have checked the boxes were ticked before pressing Save, but, really? What conceivable reason could I have for typing in a new name but not including it in the Pack & Go? I could understand if it automatically included them but gave me the option to change my mind, but this way round makes no sense.

 

SW 2016, SP5

 

 

John

By: Wayman John  Mon, 11 Dec 2017 17:11:13 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Pack & Go was torture for me for many years, for some dumb reason it took me a long long time to finally find a process that works...

By: John Stoltzfus  Mon, 11 Dec 2017 17:18:16 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

With simulation results I tried everything to have them not included in the new folder (several GB) and nothing worked...

By: Umberto Zanola  Mon, 11 Dec 2017 23:44:14 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

John Stoltzfus wrote:

 

Pack & Go was torture for me for many years, for some dumb reason it took me a long long time to finally find a process that works...

Yes, having done some more this morning, the phrase:

'As friendly as a cornered rat' comes to mind.

 

You spend 10 minutes carefully selecting and renaming all the items you want to copy, but you make a small mistake. The software points out your mistake. Excellent! Problem is, the only options are to swallow the mistake or cancel the whole process and start the ten minutes all over again. Some sort of 'Would you like to edit your selections?' button would be nice. It doesn't seem a lot to ask. Lots of software has them.

 

Someone chose to program it like that, and the checking/testing process confirmed that it was OK. Hard to understand the choices that are made sometimes.

 

Half past ten in the morning, and I am already cross. Maybe I should give it all up and become a postman or something.

 

John

By: Wayman John  Tue, 12 Dec 2017 10:33:01 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Wayman John,

 

John Wayman wrote:

 

I just spent some considerable time making a Pack & Go copy of an assembly. I needed to make new copies of less than half of the parts and re-use the remainder, so I clicked the top box to un-select all the parts first. I then typed in all the new names for the copied parts and their drawings, set the directory and clicked Save.

When I opened the new assembly, it was still using all of the old parts, because, when you type a new name in the Save To Name column of Pack & Go, it does not check the box to include that part in the Pack & Go! You then have to go back and individually check the include box for every new part and drawing.

I realise that I really should have checked the boxes were ticked before pressing Save, but, really? What conceivable reason could I have for typing in a new name but not including it in the Pack & Go? I could understand if it automatically included them but gave me the option to change my mind, but this way round makes no sense.

 

SW 2016, SP5

 

 

John

While I understand what you are saying is a frustration, this is the behavior that is expected. I have used Pack and go for the exact reasons you are using it. Since every place I have worked has an Empirical alpha numerical scheme I un-check every part then select the replace command and replace all of the numbers with the new number. Then I have to check(pick) which ones I want to bring into the new structure and which parts will not change.

 

If what you want were to be the case  I would wind up with duplicates of parts that did not actually need to be duplicated.

 

I understand why you want it to work the way you want it, I am just stating what I have seen the reasoning behind why it works the way it does.

By: Paul Risley  Tue, 12 Dec 2017 12:50:39 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Paul Risley wrote:

 

While I understand what you are saying is a frustration, this is the behavior that is expected. I have used Pack and go for the exact reasons you are using it. Since every place I have worked has an Empirical alpha numerical scheme I un-check every part then select the replace command and replace all of the numbers with the new number. Then I have to check(pick) which ones I want to bring into the new structure and which parts will not change.

 

If what you want were to be the case I would wind up with duplicates of parts that did not actually need to be duplicated.

 

I understand why you want it to work the way you want it, I am just stating what I have seen the reasoning behind why it works the way it does.

OK,

Thanks, Paul.

By: Wayman John  Tue, 12 Dec 2017 13:08:06 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

This pack and go problem.  When I would use it, (it has been a while)  I would save everything to one folder on the hard drive.  Then open the assembly and a drawing and check the file references.  If everything was pointing to the hard drive it worked out great.  Then there was the painstaking deciding of which parts where going to change and saving them to the new file name in the correct location, and replacing the files that where not going to change.

     Files that where not going to change can be deleted out of the folder and depending on how your SolidWorks search paths are set up they may show up with out you having to go and find them.  If not then there are a few to a lot of files that need to be reassociated to the assembly when you open it up.

By: David Matula  Tue, 12 Dec 2017 13:43:07 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Get this every couple of months.  A warning saying something like "your toolbar setting are inconsistent, open with default tool bar." your choice is cancel or ok.  So either I open Solidworks to fix the problem or I just leave it closed.

 

 

  Solution for me is to open then run copy setting wizard to put everything back where I like it.

By: David Nelson  Tue, 12 Dec 2017 14:46:00 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I ran into this today when creating a drawing of a part or assembly with a projected view. The right view is a projection of the left view. If both views have been selected as having custom scales (the projection is not using 'use parent scale') and then the scale of the parent view is changed, the views become misaligned. If the projected view is changed to match the scale of the parent view, they remain misaligned.  The only solution is to break alignment, and then realign by origin for each affected projection.

 

Capture.JPG

By: Colt Carson  Tue, 12 Dec 2017 14:40:09 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Oh man, now this one is really rilling me up right now.

 

When you're trying to fix an assembly because the mates are messed up, sometimes you do wrong selections and what not. Normally, you'd do a rollback by using CTRL-Z to go back to what it was but there are times where SolidWorks decides to switch the direction of a mate when you add it and when you try doing a CTRL-Z to return to the previous state, it does undo the move you did but it doesn't undo every move SolidWorks did.

 

I can't be the only one that has lost countless half hours because of SolidWorks not properly undoing what it did.

By: Alex Lachance  Tue, 12 Dec 2017 16:19:33 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Yes, Alex Lachance, you're not the only one that happens to, I've lost countless hours going back and fixing things that were flipped/deleted.

By: Edward Poole  Tue, 12 Dec 2017 16:25:40 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I feel your pain Alex, the greater frustration is that unless the offending assembly mates are replaced or supported by sketch scaffolding in sub-assemblies/parts, the erred assembly will again @show a sea of red the next time it is opened.

By: Harry Butler  Tue, 12 Dec 2017 23:20:24 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy
By: John Stoltzfus  Wed, 13 Dec 2017 11:33:22 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Let's not forget, when you undo a few steps and finally realise that SW has bypassed the step you wanted undone *grrr*, you cannot redo! Somehow SW has forgotten what it did, and you spend ages trying to retrace your steps and how far back you rolled.

 

Undo/Redo behaves like it has dementia!

By: Martin Tofts  Wed, 13 Dec 2017 11:40:08 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Here's a strange one:

I insert and mate a new part into an assembly. Concentric, Distance and Parallel mates, in this case.

I right-click the new component and select 'Copy With Mates'.

I select all the appropriate features for mating.

All works fine, but: The Distance mate is always flipped compared to the original.

I have often thought this was the case, but never analysed it. This morning, I tried it again and it seems to be repeatable. Unless I'm mistaken and it isn't...

 

SW 2016, SP5

 

John

By: Wayman John  Wed, 13 Dec 2017 11:56:25 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

That only seems to happen on drawings for me, but when it happens it can be a real pain. Thankfully most of my projects have a good start-up base so I rarely spend more then an hour on a drawing. Still, if I do spend an hour, it is annoying to lose everything because I pressed CTRL-Z and the program decided to undo every event it could undo up, which generally goes to the last save.

 

Ever since I've moved to 2016, the bug has been happening a lot less too. We will be moving to 2018 within the next months so I'm hoping that it's removed entirely in 2018

By: Alex Lachance  Wed, 13 Dec 2017 12:35:42 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I have to use Solidworks because we are a Solidworks shop and the CNC software we use (Visualmill) is a plug in for it. DO NOT like Solidworks, and here is 1 reason to start with:

In order to get proper tool paths, I often have to create sketches to drive or limit the tool. I also frequently have to make mirror image parts. If there is some way you can mirror both the part AND ITS SKETCHES in one operation, I haven't found it. Nice way to eat up time and induce error.

By: Michael McCarty  Wed, 13 Dec 2017 13:04:12 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

This isn't SolidWorks, more SolidWorks RX.

 

Every once out of 2 times I do a SolidWorks RX to send a problem to my VAR, the RX won't go through from step 2 to step 3. Here's what happens.

 

I start recording my problem, show it, finish the recording. After that, I go to upload 2 of my files on SolidWorks RX. Everything is still fine. When I press ''Package files now'', that's when the problem occurs.

 

Nothing Happens! SolidWorks RX just gets stuck there, it doesn't finish Step 2 and it doesn't move on to step 3. That's one of those things that makes me not want to send problems.

 

Edit: Just got it again, here's the screen

By: Alex Lachance  Wed, 13 Dec 2017 14:13:34 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

In a drawing of an assembly, I frequently create views with hidden lines removed, then pick and choose parts to show as needed.  This lets you have a cleaner drawing showing just what's needed vs. all of the guts in a big messy view.

 

This works well except when you want to show a sub-assembly in the view.  You can't right click on the sub in the tree and pick "show hidden component" because it won't do it if you pick the sub assembly itself.  You must pick every part in the sub assembly to get it to show up.

 

I'd like to see both options to pick the sub top level and show every part in addition to the current way where you can pick and choose which of the subs parts to show.

By: Andy Sanders  Wed, 13 Dec 2017 15:29:27 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Andy Sanders wrote:

 

In a drawing of an assembly, I frequently create views with hidden lines removed, then pick and choose parts to show as needed. This lets you have a cleaner drawing showing just what's needed vs. all of the guts in a big messy view.

 

This works well except when you want to show a sub-assembly in the view. You can't right click on the sub in the tree and pick "show hidden component" because it won't do it if you pick the sub assembly itself. You must pick every part in the sub assembly to get it to show up.

 

I'd like to see both options to pick the sub top level and show every part in addition to the current way where you can pick and choose which of the subs parts to show.

Wow, you are totally right (Sorry but I had to check to see for myself.  ).

Sub Assembly Selection:

 

Component Selection:

By: Dan Pihlaja  Wed, 13 Dec 2017 15:41:05 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Andy Sanders wrote:

 

In a drawing of an assembly, I frequently create views with hidden lines removed, then pick and choose parts to show as needed. This lets you have a cleaner drawing showing just what's needed vs. all of the guts in a big messy view.

 

This works well except when you want to show a sub-assembly in the view. You can't right click on the sub in the tree and pick "show hidden component" because it won't do it if you pick the sub assembly itself. You must pick every part in the sub assembly to get it to show up.

 

I'd like to see both options to pick the sub top level and show every part in addition to the current way where you can pick and choose which of the subs parts to show.

Andy, you should submit this in the Top Ten list.  It might not make it into the Top Ten of votes, but SWX actively logs all the TT ideas and effectively uses them as Enhancement Requests.  Actually, you should ALSO submit it as an ER.

By: Dennis Dohogne  Wed, 13 Dec 2017 15:41:32 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Added to top ten list.

By: Andy Sanders  Wed, 13 Dec 2017 15:49:38 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Andy Sanders wrote:

 

In a drawing of an assembly, I frequently create views with hidden lines removed, then pick and choose parts to show as needed. This lets you have a cleaner drawing showing just what's needed vs. all of the guts in a big messy view.

 

This works well except when you want to show a sub-assembly in the view. You can't right click on the sub in the tree and pick "show hidden component" because it won't do it if you pick the sub assembly itself. You must pick every part in the sub assembly to get it to show up.

 

I'd like to see both options to pick the sub top level and show every part in addition to the current way where you can pick and choose which of the subs parts to show.

Why don't you just use display states in the model?  If I'm poking around in the feature tree in the drawing, I'm doing something the hard way.

 

By: Jim Sculley  Wed, 13 Dec 2017 16:24:51 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I've never really warmed up to Display States.  They've been flaky (for me) when I try them.

 

In my assembly drawings, I'll typically show 2 or 3 parts while the rest of the view is HLR.  It's easy to do this on the fly.  It's either a few parts showing or everything/nothing.

 

Setting up a display state in advance to accomplish this seems like more work to me and my workflow.  Or maybe six/half dozen.

I'd rather control it at the drawing level as needed.

By: Andy Sanders  Wed, 13 Dec 2017 16:37:19 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I will second not liking the results with Display States.

By: Jim Steinmeyer  Wed, 13 Dec 2017 16:39:23 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I use the same method, didn't have good luck with display states.

By: Edward Poole  Wed, 13 Dec 2017 16:44:22 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Andy Sanders wrote:

I've never really warmed up to Display States. They've been flaky (for me) when I try them...

Andy, I use and love display states.

I design progressive tools. There is no better way (that I have found) to quickly show the "Top Half" of the tool or the "Bottom Half" of the tool. I also use it like Isolate. If I need to make a change on one particular station, I will use a display state to isolate just the details I need to make a change. The main advantage is I can save, close and come back tomorrow and get to my isolated details quick and easy.

By: Rick Becker  Wed, 13 Dec 2017 16:54:46 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Maybe I'll give them another chance sometime.

 

Whether you use Display States or not, being able to turn on hidden lines in a drawing of an entire sub-assembly at once vs. having to turn on all the parts individually would be good.

By: Andy Sanders  Wed, 13 Dec 2017 17:38:20 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Display States work well for me, and I use them often, but they're like configurations.  They can get you in trouble if you aren't careful. Especially if you don't pay attention to the Properties.

By: Glenn Schroeder  Wed, 13 Dec 2017 17:43:30 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

John Wayman wrote:

 

Here's a strange one:

I insert and mate a new part into an assembly. Concentric, Distance and Parallel mates, in this case.

I right-click the new component and select 'Copy With Mates'.

I select all the appropriate features for mating.

All works fine, but: The Distance mate is always flipped compared to the original.

I have often thought this was the case, but never analysed it. This morning, I tried it again and it seems to be repeatable. Unless I'm mistaken and it isn't...

 

SW 2016, SP5

 

John

Hi John, your experience is quite different from mine - could you be using mate to planes or sketches,rather that mate solid face to solid face. 

 

I find that copy mates to be quite predictable if the mates are solid face to solid face (because a solid face has an outside direction and an inside direction). 

 

But I do find mates plane to plane to be unstable and because the mates will often snap to the nearest solution without respecting direction, and this is true in copy mates as well as ordinary assemblies - this might be the cause of your issues and I would love to see the solidworks solver respect direction of planes when recalculating mates just like it does with faces on solid bodies - this has been a problem since before 2008. 

 

A typical example is to set a part using angle mates between planes, set the angle mate to 180 degrees and save - suppress the mate and move the part so the angle is near 0 degrees, then suppress the mate - it is not uncommon for the the mate to flip or fail.  (I normally avoid this by mating to faces a hidden solid face in a skeleton part (that in excluded from final bill of materials) when I need to get to show movements in an assembly from  from 0 to 180 degrees).

 

I suspect that much of the comment about mate errors in flexible assemblies might be related to this.

 

Ross

By: Ross Hazelwood  Wed, 13 Dec 2017 21:42:47 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Jim Wilkinson wrote:

 

Ross Hazelwood wrote:

 

Yes Jim, you are correct that we have display states linked to configurations, but that is intended and desired because we want certain configurations to look different (an example is colouring specific faces in a machined configuration to show machined faces, but the weldment would not want these).

 

Your suggested thread suggests not linking display state to configuration. However, I think you miss the main point. If display states are linked to configurations then show sketch should only show in the current display state, but the behaviour since 2010 or earlier is to show sketch in all display states. This is the fundamental error. If show sketch was fixed to operate only on the current display state (like hide sketch) then users would not have to step through every configuration to hide sketch again.

 

Hide sketch already correctly hides for the current display state only, but show sketch does not yet behave in same way.

As others have noted show/hide selected a feature but is not configurable like a feature suppress(this would be a cool improvement), but does not remove the key error that "Show sketch" is incorrectly acting on all display states while "hide sketch" is not.

Hi Ross,


What version are you using. I just tried SOLIDWORKS 2017 SP03 and 2018 SP0.1. I made a part with an extrude box and then made a sketch with a rectangle and exited the sketch. I then made a new configuration and turned on the option to have the display states linked to configurations.. I then hid the sketch switched to the other configuration and the sketch was shown there so they were independent of configuration for hiding (as you say). So I hid the sketch so it was hidden in both configurations and switched back to the other configuration. Then in the other configuration, I showed the sketch. I switched back to the other configuration and the sketch was still hidden. I tried adding a 3rd configuration and all worked as I would expect (hide/show worked independently in each configuration). I am using the Hide/Show button through the context menu on the sketch.

 

I have no doubt you are seeing something wrong, especially since two other users have agreed. I just can't reproduce it so you must be doing something differently or it is a more complex case than just a single part. Can you elaborate or try the simple case that I did to see if that is working for you? Have any of you reported it to your reseller and received an SPR?

 

Thanks,

Jim

Jim,

Like you, I cannot instantly replicate this problem so it might be part specific, or a past 2010 problem even though I describe the problem in exactly the same way as Bill Rose in Show/Hide Sketch Across Configurations 

where he states (sw2010)

"I have many parts that have multiple configurations, sometimes 20-30 configurations. When I need to make a sketch temporarily visible and select "show", the sketch is now visible in all the configurations, not just the one I'm working on. That's fine I guess, but the "Hide" portion of this command duo only works for the current config! Now I have to go into each configuration and hide that same sketch one at a time. Does this double standard have any purpose other than to make the poor user crazy? A better question is how do I hide sketches across multiple configurations without doing then one at a time? I'm fairly sure this is broken from previous releases or I would have gone nuts years ago."

 

If anyone has a example scenario and part then please post it.

 

In the meantime SW2016 SP5, I can still replicate this issue: If you have multiple configurations with display states linked to configuration - create a new sketch, then hide it, You will find it is still visible in all other configurations as expected (but not as wanted).  This revised description turns out to be a repeat of the topic of Is it possible to hide a sketch in all configurations?

 

What would be really cool is if SW provided an option to "hide in all configurations/display states" like they do with suppress features, and that is my recommendation.

 

Perhaps I or someone else could write a macro, but that requires the macro to activate every config one by one and then hide the sketch and so will be slow to execute, and I still prefer a built in option because it makes the User interface much more efficient and is a worthwhile improvement.

By: Ross Hazelwood  Thu, 14 Dec 2017 04:38:01 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Ross Hazelwood wrote:

...What would be really cool is if SW provided an option to "hide in all configurations/display states" like they do with suppress features, and that is my recommendation.

 

Nice Idea Ross. Should post that over in the SOLIDWORKS World 2018 Top Ten List.

By: Rick Becker  Thu, 14 Dec 2017 12:32:02 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Hi Dennis,

 

Showing hidden lines for sub assemblies requires selecting the component itself. That is cumbersome but okay I can go the extra mile.

What is even worse is trying to show hidden lines for individual bodies itself. In weldment part drawings you don't have access to the model cutlist body folder and you cannot select individual bodies and choose to show the hidden lines. If this body is part of a group of bodies that were created as part of a insert weldment feature, then the whole group will show the hidden lines. that is useless.

If I could show the cutlist folder in the drawing feature browser then I could select individual bodies. Why not make the cutlist folder visible in the drawing environment. Maybe SW would even allow me to preselect bodies in the drawing view to show hidden lines for the selected body only. That would be great. SW 16 couldn't do it not sure if that changed in 17 or 18.

 

 

Elmar

By: Elmar Klammer  Thu, 14 Dec 2017 12:52:36 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

All right, this one got me and I had to reach out to the VAR and have them walk me through a workaround...

In a detached drawing of a large assembly, I cannot resize the section line.  It is literally impossible.  If I click the section line, I can move the arrows but I cannot move the section line itself or resize its length to only show a portion of the assembly.  It is totally and completely broken! 

So, I reached out to the VAR and they walked me through how to edit the line in sketch mode, by turning on "Automatic Solve Mode" temporarily.

I'm sure that Alin Vargatu and Grant Mattis have run into this.  Does anyone know if there is an SPR on this?  I wasn't sure what to search for in the knowledge base on this.

In case it matters, I'm on 2017 SP3.

By: Matt Peneguy  Thu, 14 Dec 2017 14:06:11 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Elmar Klammer wrote:

 

If I could show the cutlist folder in the drawing feature browser then I could select individual bodies. Why not make the cutlist folder visible in the drawing environment. Maybe SW would even allow me to preselect bodies in the drawing view to show hidden lines for the selected body only.

Elmar

 

You should add this as an idea for 2018 top ten

By: Dan Pihlaja  Thu, 14 Dec 2017 14:11:22 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

When creating an assembly, if i set the add component dashboard to allow me to keep selecting parts to insert The open documents viewer will show both the open documents and those I have selected to insert. After I insert a part and then browse to find a second part, both parts are highlited in the viewer. Moving to the active screen will show a copy of the previous is going to be placed again. To get the correct part I click back in the viewer, it doesn't matter if I click on the previous part or the desired new part, the desired part becomes unselected and the previous part is always selected. I then have to reselect the desired new part to add it.

     I think it is actually fewer clicks to not keep the insert dashboard open.

By: Jim Steinmeyer  Thu, 14 Dec 2017 15:42:55 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

In a drawing, say you want to copy and paste one of the views.  You can change this new view to another config, scale etc.

 

Usually it goes like this:

Select view, Cntrl-C/Cntrl-V to copy it, get message "The item on the clipboard cannot be pasted here", click OK.

 

CANNOT BE PASTED HERE.jpg

 

Try Cntrl-V (again), get same message, click OK.

 

Do this again and again about 5-10 times then.....Viola!  It works and you get your copied view.

 

Why doesn't it work the very first time?!?

By: Andy Sanders  Thu, 14 Dec 2017 16:34:21 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

1-GKMRSI wrote:

 

In a drawing, say you want to copy and paste one of the views. You can change this new view to another config, scale etc.

 

Usually it goes like this:

Select view, Cntrl-C/Cntrl-V to copy it, get message "The item on the clipboard cannot be pasted here", click OK.

 

CANNOT BE PASTED HERE.jpg

 

Try Cntrl-V (again), get same message, click OK.

 

Do this again and again about 5-10 times then.....Viola! It works and you get your copied view.

 

Why doesn't it work the very first time?!?

I think you have to click somewhere within the bounds of the sheet. At least that does it for me.

By: Colt Carson  Thu, 14 Dec 2017 16:43:35 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Yep, that's what I do.  Just takes half a dozen tries.  It's not just me.  Everyone I ask here goes through the same thing.

By: Andy Sanders  Thu, 14 Dec 2017 16:46:35 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Colt Carson wrote:

 

I think you have to click somewhere within the bounds of the sheet. At least that does it for me.

As I have been building these assemblies today I have tried just clicking in the bounds and sometimes it works, other times I have to go to the view screen and make the change first.

By: Jim Steinmeyer  Thu, 14 Dec 2017 16:52:55 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

What if you select the view from the FeatureManager and CTRL-C then CTRL-V?  That's the workaround I've been using...  I'm not saying you are wrong, cut and paste should "just work", that's just the workaround I use.

By: Matt Peneguy  Thu, 14 Dec 2017 16:55:52 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Let me suggest an experiment.  When you click on a space in the drawing immediately prior to the Ctrl-V paste operation check to see if that area is in the boundary of one of the drawing views or not.  Since these boundaries are not readily apparent I suspect you might be inadvertently clicking in a view space instead of on a free area of the drawing.

By: Dennis Dohogne  Thu, 14 Dec 2017 17:10:54 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I'll give all these a shot next time I do this.  Just happened before my post so I was inspired to rant!

I usually do try to pick a "neutral" spot on the sheet (not another view border), but who knows.

By: Andy Sanders  Thu, 14 Dec 2017 17:31:51 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

This happens when you haven't clicked inside the sheet. The views on a sheet work kind of like annotations work on a view. You can bind a view to a sheet, just like you can bind an annotation to a view. For some reason, you can create views outside of the model, but if you copy and paste from one sheet to another, you have to be inside the sheet in order to copy it. I am guessing this has to do with an old setting that existed in the beginning of SolidWorks and that hasn't been updated since they expanded a drawing's limit's.

 

Edit: If it doesn't work, it's probably because you aren't binded to the sheet but the drawing. You'll know you're binded to it when the border is highlighted. See screenshots below

 

Binded to drawing:

 

Binded to sheet(Notice the pink highlight)

By: Alex Lachance  Thu, 14 Dec 2017 17:40:08 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I'm clicking in the sheet for sure. And not picking views.

I made a video of trying to copy and paste a simple view.  It took me 14 or 15 tries then it finally pasted.  I was selecting the same general spot over and over again, in the sheet and outside of any other view.

 

It would be quicker just to generate a brand new view.

 

Ccopy over and over.gif

By: Andy Sanders  Thu, 14 Dec 2017 17:57:47 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

OK, I just figured out what I'm doing wrong!

 

What I usually do is select the view, *copy*,  double click outside the view and not in any other view and inside the sheet, *paste*and I get the message it can't be copied.

 

Well, I just realized that I only should be SINGLE CLICKING in a blank spot to paste the view!  All along I was thinking that a double-click was required to make sure I was selecting the sheet.  I bet the time I was successful in pasting it, I was actually single clicking first instead of double clicking.

 

Wow, I feel dumb now!  So simple (yet so easy to do).

By: Andy Sanders  Thu, 14 Dec 2017 18:05:57 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I see your video but I don't see any highlighting of the ouside border of your sheet going on. A simple click doesn't cut it, it's usually a double click especially since I see at the beginning of the video that when you hover over your view you are binded to the view.

By: Alex Lachance  Thu, 14 Dec 2017 18:09:00 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I was selecting the view, copy, then double clicking in open space inside the drawing sheet and it was giving me the message.

 

I just discovered that all I have to do is the same exact thing, but SINGLE CLICK instead of double click to paste the view works consistently.  I plastered that circle part all over my drawing easily with the single click method.  As soon as I tried double clicking, I got the message.

By: Andy Sanders  Thu, 14 Dec 2017 18:15:04 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Well I guess it depends a bit on the pattern you follow then, my process is usually do a section on one sheet, cut the section, change sheet and double click inside sheet to paste it. Perhaps it's a little deeper like a hardware thing too, not sure though. Glad to see you figured it out though. I had that problem at the beginning and it really annoyed me so I can see where you guys are coming from.

By: Alex Lachance  Thu, 14 Dec 2017 18:21:07 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Oh how I could list many.  Start with a simple one....

 

That the measuring tool changes units and precision, if you change the units in a model or drawing.

By: Robert Adair  Thu, 14 Dec 2017 18:32:03 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

The measuring tool is made to either work with the document's settings or the settings you specify.

 

I suggest using the personalized one. I don't want to see decimal dimensions in my sketches, parts and what not. I like to have fractions when the dimension is precise and if it isn't, the dimension displays a decimal number, though when I use the dimension tool, I always want my dimensions to be taken in decimals and not fractions. When it's in decimals, I am 100% sure that it is a spot on dimension and not a rounded one.

 

Kind of like angles. I don't like seeing decimals on angles but when I do take dimensions, I want to see the decimals of the angle just to be as precise as I can be.

 

I have had some times that my tool seemed to have switched from personal settings to document settings but I think I did it without noticing because it really doesn't happen too often.

By: Alex Lachance  Thu, 14 Dec 2017 18:38:25 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Robert Adair wrote:

 

Oh how I could list many. Start with a simple one....

 

That the measuring tool changes units and precision, if you change the units in a model or drawing.

 

That's been addressed here, and is supposed to be fixed in the near future.

By: Glenn Schroeder  Thu, 14 Dec 2017 18:39:00 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Robert Adair wrote:

 

Oh how I could list many. Start with a simple one....

 

That the measuring tool changes units and precision, if you change the units in a model or drawing.

Lots of good information here that may help you: https://forum.solidworks.com/thread/211096

By: Jim Steinmeyer  Thu, 14 Dec 2017 19:24:18 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Jim Steinmeyer wrote:

 

Robert Adair wrote:

 

Oh how I could list many. Start with a simple one....

 

That the measuring tool changes units and precision, if you change the units in a model or drawing.

Lots of good information here that may help you: https://forum.solidworks.com/thread/211096

 

Thanks for posting that link Jim.  I was thinking it was in this Discussion.

By: Glenn Schroeder  Thu, 14 Dec 2017 19:30:50 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Daen Hendrickson wrote:

I tried to get a screen capture but failed. Any other clicks, Alt-Tab to switch to a different application, Ctrl-Print Screen, etc causes the condition on screen to go away...

 

 

Try just the "print screen" (without the <ctrl>.  That should save it to your clipboard.

Then try to paste to a word document or something that will take an image.

By: Rick McDonald  Fri, 15 Dec 2017 18:08:06 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Pasting copied text from a pdf into a property tab text field will show up at first but when hitting apply will delete the text. The linked property will be empty. The workaround is to strip the formatting by pasting into an intermediate program like notepad, then copy and paste the text from there.

 

text from pdf.JPG

By: Colt Carson  Fri, 15 Dec 2017 18:38:58 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Colt Carson wrote:

 

Pasting copied text from a pdf into a property tab text field will show up at first but when hitting apply will delete the text. The linked property will be empty. The workaround is to strip the formatting by pasting into an intermediate program like notepad, then copy and paste the text from there.

 

text from pdf.JPG

I could be wrong, but I believe that this only happens with multi-line text.  If you paste each line individually into 1 line, then I think it will work.

By: Dan Pihlaja  Fri, 15 Dec 2017 18:43:55 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Rick McDonald wrote:

 

Daen Hendrickson wrote:

I tried to get a screen capture but failed. Any other clicks, Alt-Tab to switch to a different application, Ctrl-Print Screen, etc causes the condition on screen to go away...

 

 

Try just the "print screen" (without the <ctrl>. That should save it to your clipboard.

Then try to paste to a word document or something that will take an image.

Or download Greenshot.

http://getgreenshot.org/

By: Dan Pihlaja  Fri, 15 Dec 2017 18:47:11 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Dan Pihlaja wrote:

 

Rick McDonald wrote:

 

Daen Hendrickson wrote:

I tried to get a screen capture but failed. Any other clicks, Alt-Tab to switch to a different application, Ctrl-Print Screen, etc causes the condition on screen to go away...

 

 

Try just the "print screen" (without the <ctrl>. That should save it to your clipboard.

Then try to paste to a word document or something that will take an image.

Or download Greenshot.

http://getgreenshot.org/

+1 on GreenShot. Great program.

By: Tony Tieuli  Fri, 15 Dec 2017 18:55:37 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Daen Hendrickson wrote:

 

I am using SW2014 SP5.

 

While trying to resize a plane by clicking and then dragging the displayed grab handles, you cannot get the "double arrow" mouse pointer (indicating resize) when you hover over a grab handle while the pop-up shortcut toolbar is visible (sorry, can't recall the proper name). You must first click elsewhere to extinguish the pop-up (or press esc, ctrl, or alt or ???). Maybe not expressly a "bug" but certainly an unnecessary extra click.

 

I tried to get a screen capture but failed. Any other clicks, Alt-Tab to switch to a different application, Ctrl-Print Screen, etc causes the condition on screen to go away...

 

Daen

I would add that I would like the "Autosize" command with planes other than the first 3.

By: Jim Steinmeyer  Fri, 15 Dec 2017 19:07:09 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Jim Steinmeyer wrote:

I would add that I would like the "Autosize" command with planes other than the first 3.

Hi Jim,

 

All planes do autosize by default. However, user created planes don't resize to the bounding box of the model (like the default planes), but rather to the geometry that created the plane. For instance, create a plane using 3 points and the plane will be sized based on the location of the 3 points (slightly larger than a rectangle bounding the 3 points). Drag to resize that plane you just made and then right mouse button on the plane and you can select Autosize and it will go back to being sized based on the 3 points. If the model changes such that the 3 points move, the plane will resize to the new position of the 3 points.

 

Perhaps you want an option to autosize user created planes to the model bounding box instead? If so, I would suggest submitting an enhancement request.

 

Thanks,

Jim

By: Jim Wilkinson  Fri, 15 Dec 2017 19:18:01 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Jim Wilkinson

Yes you are correct, I would like it to size to the bounding box. But I did learn something new, I was unaware you could Autosize it back to the size it started at.

 

Thank you

By: Jim Steinmeyer  Fri, 15 Dec 2017 19:31:21 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I am using SW2014 SP5.

 

While trying to resize a plane by clicking and then dragging the displayed grab handles, you cannot get the "double arrow" mouse pointer (indicating resize) when you hover over a grab handle while the pop-up shortcut toolbar is visible (sorry, can't recall the proper name). You must first click elsewhere to extinguish the pop-up (or press esc, ctrl, or alt or ???). Maybe not expressly a "bug" but certainly an unnecessary extra click.

 

I tried to get a screen capture but failed. Any other clicks, Alt-Tab to switch to a different application, Ctrl-Print Screen, etc causes the condition on screen to go away...

 

Daen

 

EDIT: Image added per Jim Steinmeyer's suggestion

 

By: Daen Hendrickson  Fri, 15 Dec 2017 16:00:48 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

In Extrude Features using a 'From' offset

This is a minor annoyance I always forget about... the dimension placement breaks when you edit a dimension.

From my brief test if you edit the feature the dims return to the correct spot

 

SW16 SP5

 

 

 

 

 

 

 

edit: the draught angle doesn't care either way

By: Rob Edwards  Sat, 16 Dec 2017 12:28:00 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I consider this a bug:

The above just means 4 x 3/4" THRU!

It should not be possible to specify a slot length that is smaller than the hole!  I was terribly confused when I opened a part with a slot like this:

Is this a known thing, anyone know of an SPR on this?

By: Matt Peneguy  Sun, 17 Dec 2017 16:19:52 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

When creating custom views for a drawing I often run into the problem where the orientation tool does not give the expected result.

 

ISO1.JPG

The the view normal direction is correct but the view is rotated by 30 degrees.

 

RESULT.JPG

By: Colt Carson  Mon, 18 Dec 2017 15:41:37 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

so that is the bug?

 

# 1 learn to update and rest the standard views... than your problems will tend to go away.

#2 there if very little reason to have to create any custom view for a simple part the top front and right views should be more than enough for the part that you shown.

#3 start the part on the right plane will lead to better times on the drawing,

By: David Matula  Mon, 18 Dec 2017 16:02:23 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

David Matula wrote:

 

 

#3 start the part on the right plane will lead to better times on the drawing,

David, I never heard of such a thing.  What supports this comment?

By: Dennis Dohogne  Mon, 18 Dec 2017 16:14:03 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

I appreciate you suggestions and have done such things as updating the standard views to get the views I want. The displayed part was just used to show the problem. Sometimes in a very complex assembly we need to show many iso views from more than just one angle to clarify the assembly process.  Also they asked for simple bugs, this one that I encounter relativity often should be easy for an intern to address.

By: Colt Carson  Mon, 18 Dec 2017 16:18:00 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Dennis Dohogne wrote:

 

David Matula wrote:

 

 

#3 start the part on the right plane will lead to better times on the drawing,

David, I never heard of such a thing. What supports this comment?

Zero, Zero, Zero - 0,0,0 -

By: John Stoltzfus  Mon, 18 Dec 2017 16:27:27 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

Colt Carson wrote:

 

Also they asked for simple bugs, this one that I encounter relativity often should be easy for an intern to address.

I just want to make clear that this thread was started by a user, not by SOLIDWORKS. So it is not a thread for officially reporting problems to SOLIDWORKS. For that, you need to use your regular support channel (which for most users is their reseller).

 

I am going to lock this thread because:

  1. It is giving the false impression to users that this is where they should report minor problems.
  2. The thread is so long and unwieldy, it is impossible to find anything in it and very difficult to follow.

 

If users want to report problems in the forum to get other users to suggest workarounds or something like that, it is important to post each item as a separate thread in the "space" in the forum specific to the problem being reported. That way, both users and SOLIDWORKS employees who monitor the different spaces of the forum because they are experts in that area will see it rather than it being buried in the General section in a 55 page thread.


Thanks,

Jim

By: Jim Wilkinson  Mon, 18 Dec 2017 16:34:29 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

John Pesaturo wrote:

 

More of an annoyance than a bug but all the same ...

 

It makes me nuts how the cursor/pointer jumps off of the origin when trying to drop a part on the Origin in an assembly.

 

SW2017 SP 2.0

Hi John,

 

This problem has been fixed in SOLIDWORKS 2018 SP02.

 

Thanks,

Jim

By: Jim Wilkinson  Wed, 07 Mar 2018 11:31:55 GMT
Re: What *Minor* Bug in SOLIDWORKS Drives You Crazy

1-9DBF56 wrote:

 

Jim Steinmeyer wrote:

 

Jim,

Actually, my problem is more along the lines that SW forgets that I have selected the first quadrent. I pick a radius while holding the shift and the whole radius highlights for a second or two. Often by the time I get to the second radius the first is no longer highlighted so when I select the second it is just like I am starting over. As John Stoltzfus has said many times it may be that I am doing something wrong, So I will try it again a few times today and see if it works better if I am more deliberate in my selections.

 

Thank you

Hi Jim,


Sorry about the delay. I was out of the office quite a bit and needed to test older versions in the office to fully test this. It is logged as SPR# 955110 and this link should go to it in the Knowledge Base:

https://customerportal.solidworks.com/eservice_enu/start.swe?SWECmd=InvokeMethod&SWEMethod=GotoRecord&SWEService=SWGotoR…

If any users are facing issues using shift dimension to dimension between arc extents and the first selection "randomly" dropping before you can pick the second one, please either select the option it the KB to indicate you want to be notified when it is fixed or contact your reseller and ask them to attach you to the SPR.

 

Thanks,

Jim

Hi Everyone,

 

This problem of dimension in drawings while using the shift key randomly dropping the first selection which was logged as SPR# 955110 is fixed in SOLIDWORKS 2018 SP02.

 

Thanks,

Jim

By: Jim Wilkinson  Wed, 07 Mar 2018 12:00:54 GMT
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