FAQ - Part 2
SOLIDWORKS Forums
3 days ago

Frequently Asked Forum Questions (see attached PDF) has 25 topics, and I think that's enough without it getting too difficult to navigate, so I'm starting a new one.  To avoid confusion I'll start here with #26.  I'll add to and edit this periodically, and if you see a mistake or have a suggestion please send me a Private Message.  I really hate typos.

 

26.  Saving document settings

27.  SW on a Mac

28.  Placing holes on a cylinder or cylindrical surface

29.  Drawing dimension lost reference

30.  Using an Equation or Global Variable in a feature

31.  What does this icon mean?

32.  Can I get some help with my schoolwork?

33.  Moving sketch from Assembly to Part

34.  Dimensioning to the intersection of two edges

35.  Saving a Drawing or Assembly to make changes

36.  Using one Part to remove material from another one in an Assembly

37.  Removing unwanted Part from new Assembly

 

   26.  I've made some changes to a Part at Tools > Options > Document Properties, but when I start a new Part it reverts to the default settings.  How can I use those in a new Part?

   (Before I get started, the instructions I'm giving here apply to Parts, but the process is the same for Assemblies and Drawings.)

   Open a new blank Part and make the desired changes.  Go to File > Save, and choose Part Templates (*.prtdot) from the drop-down at "Save as type:".

 

   Name the file appropriately and save.  I'd strongly suggest saving it somewhere other than the default location in the SolidWorks installation folder so you won't lose it if you upgrade to a newer version.  If you're in a multi-user environment you might want to save it to a network so it's available for other users.  Next go to Tools > Options > System Options > File Locations > Document Templates.

 

 

   Click on the "Add..." button, browse to the folder where you saved the template, and select it.  I'd suggest deleting the default location that's there now, but that's up to you.  Now when you start a new Part you should have the new template available to choose from.  If you don't, and you see this...

 

 

...which only has the default templates to choose from, click on the "Advanced" button at lower left.  Then it should look something like this:

 

 

You only see one Part and one Assembly template here because that's all I need.  Depending on your needs you can certainly have more.  Just name them appropriately so you know what you're choosing.  If you have a large number of document templates you can add sub-folders at the location you're pointing to at File Locations > Document Templates and these sub-folders will show up as tabs in the Advanced New Document dialog box.  See above.  "Templates" is my main folder that contains all my templates, and "Other Drawings" is a sub-folder.  It contains some drawing templates that I rarely use but don't want to get rid of.

   While I'm on the subject, occasionally someone will ask how to apply new Document Property settings to an existing document.  You can open a document with the desired settings, go to Tools > Options > Document Properties > Drafting Standard, and select "Save to External File...".  Save this standard, then open the existing document, go to the same location, choose "Load From External File..." and Browse to and select the desired saved standard.  I haven't used this much, and have gotten mixed results when I did, but it's worth a shot.  Another option, for Drawings, is to open the existing Drawing, then start a new one with the new Template, and copy sheets from the existing document and paste them into the new one.  This isn't a perfect procedure either, but one I've used with some success.

 

 

   27.  Can I use SolidWorks with my Mac computer, or does it only run on Windows?

   See the reply from Anna Wood at what is the best way to run SW on a Mac laptop? I have nothing to add as I have exactly zero experience with Apple products.

 

   28.  I want to place some holes on the surface of a cylinder.  How do I do that?

   If you need simple round holes, slots, or any other type that can be made with the Hole Wizard feature, it's pretty simple.  Sketch points placed on the surface of a cylinder using Hole Wizard will automatically be placed with the holes perpendicular to the cylinder's axis.  For any other shape I'd suggest creating a plane and then use this for a 2d sketch just like you'd do for placing holes on a flat surface.  You'll need two references to fully define the new plane.  The simplest is to use the cylindrical surface (Tangent) and another plane (Parallel, Perpendicular, etc).  If using an existing plane doesn't work then you'll probably need to create a sketch and use one of its entities (line, point, etc.) for the second reference.

 

   29.  I made some changes to my model, and when I went back to the Drawing one (or some) of the dimensions have turned an ugly yellowish-brown color.  What happened and how can I fix it?

   That's referred to as a "dangling dimension", meaning it's lost its reference to the model  Either it was referencing something that's no longer there, or something that's moved, or maybe your computer just hiccuped.  If it had referenced a feature that was deleted then you'll obviously need to click on the dimension and delete it.  If its reference just moved, you should be able to re-attach it.  Click on the dimension to highlight it.  There should be a small red box at the end of an extension line.

 

 

   You should be able to click on it and drag it to the new reference.  Keep in mind that you can only re-attach it to the same type of reference that was used to create the dimension.  For example, if a model edge was used to create the dimension then you won't be able to re-attach it to a point or vertex.  If you can't get it to re-attach, which sometimes happens, just delete the dimension and use the Smart Dimension tool to insert a new one.  Occasionally a dangling dimension will appear to not be selectable (won't turn blue when you click on it), but when that happens I've always been able to click on it anyway and delete it with the Delete key on my keyboard.  I've also run into a situation a time or two when a dimension would turn that color and appear to have lost it's references, but would be all blue when I clicked on it instead of having the red box.  This seems to happen mostly when copying and pasting sheets from one drawing to another.  When that happens I can still click on the box at the end of the extension line and re-attach it.

   While I'm on the subject, notes and balloons (and other annotations) will sometimes lose their reference also and turn that same color.  When that happens just click the end of the leader and re-attach it.

   There's a setting you can choose that will automatically hide these annotations, but I keep it turned off.  If there's a problem with an annotation I want to know about it.  If it just goes "poof" I very likely might not notice.

 

 

   30.  I have a Global Variable (or Custom Property, etc) that I'd like to link to in a Linear Pattern, Distance Mate, or similar feature that contains a dimension.  Is this possible?

   Yes.  Some features, such as Linear Component Patterns in Assemblies, allow the use of Equations directly in the Property Manager (just type the Equal sign in the dimension dialog box, see below), but this was added fairly recently, so may not be available if you're using an earlier version, and still isn't available for all features.

 

   If you can't do it directly in the Property Manager, go ahead and create the feature, using a dimension that's close to what you need.  Click Okay to close the feature, then single-click on it in the tree to show the dimension in the graphics area (or double-click if you don't have Instant 3d turned on).

 

 

   Double-click on it to bring up the standard dimension dialog box, enter the Equal sign, and link to your variable, custom property, etc.  You'll need to do a manual rebuild for the change to take effect.

 

 

   31.  I have an icon in my tree that I don't recognize.  What does it mean?

   Please see this blog post from Jim Wilkinson.  It shows all the icons (or almost all; if you have one you don't see there please let him know), along with links to SW Help for each group.

 

   32.  I'm having problems with a school assignment.  Can someone help please?

  I, or someone else, will be glad to help.  Most of us here enjoy helping others learn more about SolidWorks, and some active forum members are teachers.  If you want help learning then please post your specific question about what part of your assignment you're having trouble with.  Include screenshots of your work at a minimum, and attaching your model will be better.  More and better information will get you more and better answers.

   If, on the other hand, instead of help you want someone to do your work for you, please don't bother asking.  It's dishonest, and you won't learn anything that way.

 

   33.  I have a sketch that was created in my Assembly, and I'd like to move it to one of the Parts in the Assembly.  Can I do that?

   There isn't a way to do that directly, but there are at least two methods that should work for you.  You can copy the sketch from the Assembly and paste it into the Part file, then delete it from the Assembly.  You will need to reapply some relations to fully define it in the Part.  Another option would be to edit the Part within the Assembly, create a new sketch on the same plane as the Assembly sketch (or one that's parallel to it), and use the "Convert Entities" sketch tool to reproduce the sketch entities in the Part.  If you use this option you will of course need to keep the sketch in the Assembly instead of deleting it, unless you first delete the "On Edge" relations.

 

   34.   How do I dimension to the intersection of two edges, such as at a chamfer or fillet?

   With the Smart Dimension tool active, right-click on one of the edges and choose "Find Intersection" from the drop-down.

 

 

Then click on the second edge.  That will insert a Virtual Sharp at the intersection of the two edges, and establish it as the dimension reference.  This right-click option is a fairly recent enhancement (SW2015, maybe?).  If you're using an older version, then exit the Smart Dimension function, Ctrl+select the two edges, and then select the Point sketch tool.  That will place a Virtual Sharp at the intersection of the edges, and now you can dimension to it.  By the way, you can choose which of several styles you prefer for Virtual Sharps at Tools > Options > Document Properties > Virtual Sharps.

 

 

Unfortunately, there isn't currently (as of SW2017) a way to set a Layer or color for them.  You can use a Layer to change the color if you don't like the default.

 

 

   35.   I have an Assembly (or Drawing), and now I want a new one that's very similar.  What's the best way to do that without messing up the original?

With the parent file open, go to File > Pack and Go.  That will allow you to copy the file, and all of its dependent files (Parts, sub-assemblies, etc.) to another location.  Most of the options are self-explanatory, but I'll touch on a couple of them.  If you use Toolbox, there's a box near the top left you can de-select to avoid copying them.  There's also an option near the bottom left to send the files to a Zip file, which is handy if you need to send them to someone (or post them in a forum).

 

Changing the names of the new files is a good policy to make sure you don't get unintended changes to your original files.  There are three ways to do this:

   1.  Double-click on the file name in the "Save to Name" column.  That will allow you to assign a new name to individual files.  This works fine if there aren't too many files, but for those with quite a few use 2 or 3.

   2.  There are checkboxes near the bottom right corner where you can add a suffix or prefix to the new file names.

   3.  Use the "Select / Replace" button (near the center, just below the list of files) to replace text in file names (such as project numbers) with new text.  This function can also be used to exclude some components (such as library parts) by selecting "In Folder" from the Search drop-down, entering a key word, and then selecting "Uncheck item(s)".

 

When you've finished and clicked "Save", be sure to close your original file (I learned this the hard way), then open the new files to make your changes.

 

 

   36.   I have one Part interfering with another one in an Assembly and I want to use the interference to remove material from one of them.  How do I do that?

In the Assembly, click on the one you want to cut and choose the "Edit Part" icon.  That will allow you to edit this Part in the context of the Assembly.

 

 

Now choose the Indent command (Insert > Features > Indent).  Select the Part you want to cut ("Target body:") and the Part you want to cut it with (Tool body region:), and choose "Cut".

 

 

Click on the Okay icon and you're done.

 

 

   37.   When I start a new Assembly there is a Part (or Parts, or a sketch, etc) already there that I don't want.  What happened, and how do I fix it?

Somehow your Assembly Template got saved with the Part in it.  Possibly you (or someone) started a new Assembly, made some changes at Tools > Options > Document Properties, and saved the template after this Part had been inserted.  How it happened doesn't really matter, but it's easy enough to fix.  Start a new Assembly with this template, delete the Part, and then File > Save as > Assembly Template.   Saving it to the same name will override the template with the Part already inserted, or save it to a new name.


Categories: General

Comments
Last comment By: Glenn Schroeder   Tue, 12 Dec 2017 17:39:44 GMT
Re: FAQ - Part 2

Great work Glenn

 

I would suggest to create the PDF and attach to main post; like I've done in this one Forum Posting

By: Deepak Gupta  Wed, 11 Jan 2017 16:51:00 GMT
Re: FAQ - Part 2

Deepak Gupta wrote:

 

Great work Glenn

 

I would suggest to create the PDF and attach to main post; like I've done in this one Forum Posting

 

Done.  Thank you for the suggestion.

By: Glenn Schroeder  Wed, 11 Jan 2017 16:58:55 GMT
Re: FAQ - Part 2

#29 some Dangling Dims will not delete.  That is the only time I will used the Hide the Dangling Dims option.  I would rather  they be gone.

By: David Nelson  Wed, 25 Jan 2017 22:26:10 GMT
Re: FAQ - Part 2

Glenn, you skipped Question 31.

 

31.  Determining what version was last used to save a file

By: Dan Pihlaja  Fri, 17 Feb 2017 13:12:19 GMT
Re: FAQ - Part 2

Thanks Dan.  While I was working on this I decided that that information might fit better added onto #3 at the original FAQ, but forgot to fix the list at top here.  I have now done so.

By: Glenn Schroeder  Fri, 17 Feb 2017 13:34:06 GMT
Re: FAQ - Part 2

Glenn, I'm still open to coming to College Station and helping you get a User Group started.  It's a shame you don't run one with all this knowledge stored up.  I'm sure Richard Doyle would love another user group in Texas

 

BTW, I met an A&M fellow at World and invited him to come down to Austin (really Round Rock) to our next meeting, you're welcome to come, too.

 

Steve C

By: Steve Calvert  Fri, 17 Feb 2017 13:38:37 GMT
Re: FAQ - Part 2

Thank you for the offer.  I'm willing to help get one going here if Richard thinks it's a good idea.  And thank you for the invitation.  I'd like to come to one of your meetings.

By: Glenn Schroeder  Fri, 17 Feb 2017 14:05:14 GMT
Re: FAQ - Part 2

Added 32.  I'm having problems with a school assignment.  Can someone help please?

By: Glenn Schroeder  Thu, 23 Mar 2017 19:55:43 GMT
Re: FAQ - Part 2

Forgot where I read it. But if you click on a Dangling Dim and it does not Highlight try hitting Delete key anyway.  99% of the time it will disappear. so I no longer need to hide them.  Hated doing that.

By: David Nelson  Thu, 23 Mar 2017 20:58:44 GMT
Re: FAQ - Part 2

Thank you Glenn!   I hope you don't mind that I am going to totally reference this to others, like.....all the time......I will give you kudos though!

By: Dan Pihlaja  Fri, 24 Mar 2017 11:57:18 GMT
Re: FAQ - Part 2

David Nelson wrote:

 

Forgot where I read it. But if you click on a Dangling Dim and it does not Highlight try hitting Delete key anyway. 99% of the time it will disappear. so I no longer need to hide them. Hated doing that.

 

Maybe you read it right here?

 

By: Glenn Schroeder  Fri, 24 Mar 2017 12:13:50 GMT
Re: FAQ - Part 2

Dan Pihlaja wrote:

 

Thank you Glenn! I hope you don't mind that I am going to totally reference this to others, like.....all the time......I will give you kudos though!

 

I don't mind at all.  I'm flattered that you think it's worth passing along.

By: Glenn Schroeder  Fri, 24 Mar 2017 12:14:19 GMT
Re: FAQ - Part 2

Glenn Schroeder, I have a simple request.  When you make an edit to either of these FAQs please go to the bottom of the post after making the edit and telling us what you changed.  I have gone to these posts because I see that there has been new activity and it turns out you edited something, but I cannot tell what change you made.

 

Thanks for putting together such helpful information!!

By: Dennis Dohogne  Fri, 24 Mar 2017 15:03:21 GMT
Re: FAQ - Part 2

You need to add a revision column...... 

By: Dan Pihlaja  Fri, 24 Mar 2017 15:04:52 GMT
Re: FAQ - Part 2

Dennis Dohogne wrote:

 

Glenn Schroeder, I have a simple request. When you make an edit to either of these FAQs please go to the bottom of the post after making the edit and telling us what you changed.

 

Sometimes it's just re-wording, so no information was added, but lately I've added a comment at the end if there was a more substantive edit (like the screenshot below from yesterday).  Will that work?

 

By: Glenn Schroeder  Fri, 24 Mar 2017 15:24:23 GMT
Re: FAQ - Part 2

Yep, that would be perfect.  If there is no comment at the bottom and the most recent post from you is tied to your OP then I'll assume it is only something like minor rewording.

 

Thanks!!!!!

By: Dennis Dohogne  Fri, 24 Mar 2017 16:28:29 GMT
Re: FAQ - Part 2

Added    33.  I have a sketch that was created in my Assembly, and I'd like to move it to one of the Parts in the Assembly.  Can I do that?

By: Glenn Schroeder  Wed, 29 Mar 2017 18:19:57 GMT
Re: FAQ - Part 2

If possible, I wanted to point one thing out:

When you are selecting a sketch using the "convert entities" method, then make sure that you are selecting the sketch from the hierarchy tree, unless you want to use only specific lines/arcs from the sketch.

 

The reason for this is that, if you select the sketch from the tree, it grabs the sketch as a whole....and if you later remove lines/arcs from the sketch, then it will still work in your extrude or whatever you are using it for without errors (unless you leave gaps).   If you select individual lines/arcs instead, and you later remove some of them, then you will have errors later.

By: Dan Pihlaja  Wed, 29 Mar 2017 18:35:03 GMT
Re: FAQ - Part 2

John Stoltzfus, I think you need to clarify how this statement fits with your advocating the use of layout/skeleton sketches (for those that don't immediately see the difference, that is  ).

By: Dennis Dohogne  Wed, 29 Mar 2017 19:07:40 GMT
Re: FAQ - Part 2

Looks like you were editing to incorporate that as I was typing that suggestion.  Good job!

By: Dennis Dohogne  Wed, 29 Mar 2017 19:08:39 GMT
Re: FAQ - Part 2

FYI (something that I learned the other day):

 

 

I am not trying to say that what John Stoltzfus is saying isn't valid, because it is.....I am just pointing it out that it is possible to create a sketch that is first in the tree in the assembly.

By: Dan Pihlaja  Wed, 29 Mar 2017 19:12:25 GMT
Re: FAQ - Part 2

Thanks for getting this together Glenn Schroeder - I do want to mention that sketches in Assemblies just came up this week here on the forum, I'm talking about sketches in the Assembly File not a part of just sketches...  The way SW rebuilds having a sketch in the assembly level can be a culprit for circular rebuild issues, especially if that same sketch is driving other components.

 

So the best way is to eliminate any sketches, in the Assembly if it's used to control sub-assemblies and part features, I don't mean Skeleton Sketch Parts or parts that have sketches in them, SW starts at the top of the feature tree and works it's way down and if a part has a feature that uses an Assembly Sketch, which btw is at the bottom of the feature tree.  I actually have a few older assemblies like that, so I'll be checking them out, they just don't rebuild cleanly...

 

EDITED: Thanks Dan Pihlaja - for bringing up the post below -  That is correct - "If" you add the Sketch before any part then it's what Frank Ruepp says, but if the sketch is an after thought then that's where my blah blah is focusing on  - Thanks again Dan

By: John Stoltzfus  Wed, 29 Mar 2017 18:52:04 GMT
Re: FAQ - Part 2

There's sooo much to soak up, first the new people need to get past #32 - lol  -  An advocate??? Just somebody that has a workflow that happens to work for what he does..........

 

So - to verify the difference

 

1. A Skeleton Sketch Part is a virtual part that controls the entire assembly and it's position needs to be the first part in the feature tree, that way it get's rebuilt first and is clean and ready..

 

2.  The other sketch I'm talking about is when you're in an assembly and you decide that you need to put in some bearing holes, instead of editing the part, you click on the face of the plate, insert a sketch, and use the cut-extrude feature with the little box checked propagate to the part file, with a dialog box allowing you to include all or any of the parts in the feature tree.  This can be a rebuild killer, because the rebuild process starts at the top of the feature tree and works down, so the hole you just cut in plate 2 and 4 can't be cleanly rebuilt before the sketch, which btw is the last in the feature tree and needs to reach back up to rebuild plate 2 & 4, and it only gets worse if you use the hole in plate 4 to control a feature in plate 6 and 2....

By: John Stoltzfus  Wed, 29 Mar 2017 19:19:00 GMT
Re: FAQ - Part 2

John,

 

This may be a dumb question, but that hasn't stopped me before.  Why do you have a Skeleton Sketch Part controlling the other Parts instead of just a sketch in the Assembly?

By: Glenn Schroeder  Wed, 29 Mar 2017 19:46:30 GMT
Re: FAQ - Part 2

Not a dumb question at all -

 

That same Skeleton Sketch Part is first part in the Main Assembly and also the first part in "Every" Sub-Assembly, which makes it a transferable part.  What this does is allow the assembly to be broken down to zones and you can work on the sub-assembly and actually complete all the detail in that assembly and never have to open the Main Assembly or any of the other Sub-Assemblies..

 

If just a normal sketch is in the assembly top or bottom of the feature tree, that's where it stays, unless you put that assembly in side of another assembly, which would then change it's terminology to a Skeleton Sketch Assembly

 

If you have simple assembly then it would be the best to insert a sketch in the assembly file "Before" any parts are inserted...

 

EDITED -

 

Glenn Schroeder - interesting and an exciting find see my reply to Frank Ruepp here - https://forum.solidworks.com/thread/202725#729805

 

If you have a folder in your assembly template and in that folder you have just one sketch you can add sketches and be able to drag and drop them into the the folder even after you insert parts into the assembly, this is really an important step to take in creating or updating your assembly templates, because of the rebuild sequence that SW uses...

By: John Stoltzfus  Wed, 29 Mar 2017 19:58:14 GMT
Re: FAQ - Part 2

Added  #34.  Dimensioning to the intersection of two edges

By: Glenn Schroeder  Tue, 09 May 2017 18:25:54 GMT
Re: FAQ - Part 2

Glenn Schroeder wrote:

 

Added #25, about using Pack and Go.

#35.  You had me looking elsewhere there for a minute. 

By: Dennis Dohogne  Wed, 05 Jul 2017 20:13:08 GMT
Re: FAQ - Part 2

Glenn, I'd like to suggest adding something along these lines to #35:

 

There are several options there in the Pack and Go that are very handy as well as some very handy summary information (circled in blue).  If someone is just learning about Pack and Go it would serve them well to really look into it to see how to exploit the options available:

 

Don't forget to hit the Help button while there to easily learn more.

By: Dennis Dohogne  Wed, 05 Jul 2017 20:27:19 GMT
Re: FAQ - Part 2

Added #25, about using Pack and Go.

 

Edit:  That should be #35, not #25.

By: Glenn Schroeder  Wed, 05 Jul 2017 19:57:54 GMT
Re: FAQ - Part 2

Added:

 

36.  Using one Part to remove material from another one in an Assembly

By: Glenn Schroeder  Fri, 15 Sep 2017 14:36:13 GMT
Re: FAQ - Part 2

If you "Edit" the part you can also use the "Cavity" Feature..

By: John Stoltzfus  Fri, 15 Sep 2017 15:06:55 GMT
Re: FAQ - Part 2

Added:

 

37.   When I start a new Assembly there is a Part (or Parts) already there that I don't want.  What happened, and how did I fix it?

By: Glenn Schroeder  Wed, 22 Nov 2017 13:51:56 GMT
Re: FAQ - Part 2

2017-11-29:  Minor edit to #30.

By: Glenn Schroeder  Wed, 29 Nov 2017 14:44:42 GMT
FAQ - Part 2

Frequently Asked Forum Questions (see attached PDF) has 25 topics, and I think that's enough without it getting too difficult to navigate, so I'm starting a new one.  To avoid confusion I'll start here with #26.  I'll add to and edit this periodically, and if you see a mistake or have a suggestion please send me a Private Message.  I really hate typos.

 

26.  Saving document settings

27.  SW on a Mac

28.  Placing holes on a cylinder or cylindrical surface

29.  Drawing dimension lost reference

30.  Using an Equation or Global Variable in a feature

31.  What does this icon mean?

32.  Can I get some help with my schoolwork?

33.  Moving sketch from Assembly to Part

34.  Dimensioning to the intersection of two edges

35.  Saving a Drawing or Assembly to make changes

36.  Using one Part to remove material from another one in an Assembly

37.  Removing unwanted Part from new Assembly

 

   26.  I've made some changes to a Part at Tools > Options > Document Properties, but when I start a new Part it reverts to the default settings.  How can I use those in a new Part?

   (Before I get started, the instructions I'm giving here apply to Parts, but the process is the same for Assemblies and Drawings.)

   Open a new blank Part and make the desired changes.  Go to File > Save, and choose Part Templates (*.prtdot) from the drop-down at "Save as type:".

 

   Name the file appropriately and save.  I'd strongly suggest saving it somewhere other than the default location in the SolidWorks installation folder so you won't lose it if you upgrade to a newer version.  If you're in a multi-user environment you might want to save it to a network so it's available for other users.  Next go to Tools > Options > System Options > File Locations > Document Templates.

 

 

   Click on the "Add..." button, browse to the folder where you saved the template, and select it.  I'd suggest deleting the default location that's there now, but that's up to you.  Now when you start a new Part you should have the new template available to choose from.  If you don't, and you see this...

 

 

...which only has the default templates to choose from, click on the "Advanced" button at lower left.  Then it should look something like this:

 

 

You only see one Part and one Assembly template here because that's all I need.  Depending on your needs you can certainly have more.  Just name them appropriately so you know what you're choosing.  If you have a large number of document templates you can add sub-folders at the location you're pointing to at File Locations > Document Templates and these sub-folders will show up as tabs in the Advanced New Document dialog box.  See above.  "Templates" is my main folder that contains all my templates, and "Other Drawings" is a sub-folder.  It contains some drawing templates that I rarely use but don't want to get rid of.

   While I'm on the subject, occasionally someone will ask how to apply new Document Property settings to an existing document.  You can open a document with the desired settings, go to Tools > Options > Document Properties > Drafting Standard, and select "Save to External File...".  Save this standard, then open the existing document, go to the same location, choose "Load From External File..." and Browse to and select the desired saved standard.  I haven't used this much, and have gotten mixed results when I did, but it's worth a shot.  Another option, for Drawings, is to open the existing Drawing, then start a new one with the new Template, and copy sheets from the existing document and paste them into the new one.  This isn't a perfect procedure either, but one I've used with some success.

 

 

   27.  Can I use SolidWorks with my Mac computer, or does it only run on Windows?

   See the reply from Anna Wood at what is the best way to run SW on a Mac laptop? I have nothing to add as I have exactly zero experience with Apple products.

 

   28.  I want to place some holes on the surface of a cylinder.  How do I do that?

   If you need simple round holes, slots, or any other type that can be made with the Hole Wizard feature, it's pretty simple.  Sketch points placed on the surface of a cylinder using Hole Wizard will automatically be placed with the holes perpendicular to the cylinder's axis.  For any other shape I'd suggest creating a plane and then use this for a 2d sketch just like you'd do for placing holes on a flat surface.  You'll need two references to fully define the new plane.  The simplest is to use the cylindrical surface (Tangent) and another plane (Parallel, Perpendicular, etc).  If using an existing plane doesn't work then you'll probably need to create a sketch and use one of its entities (line, point, etc.) for the second reference.

 

   29.  I made some changes to my model, and when I went back to the Drawing one (or some) of the dimensions have turned an ugly yellowish-brown color.  What happened and how can I fix it?

   That's referred to as a "dangling dimension", meaning it's lost its reference to the model  Either it was referencing something that's no longer there, or something that's moved, or maybe your computer just hiccuped.  If it had referenced a feature that was deleted then you'll obviously need to click on the dimension and delete it.  If its reference just moved, you should be able to re-attach it.  Click on the dimension to highlight it.  There should be a small red box at the end of an extension line.

 

 

   You should be able to click on it and drag it to the new reference.  Keep in mind that you can only re-attach it to the same type of reference that was used to create the dimension.  For example, if a model edge was used to create the dimension then you won't be able to re-attach it to a point or vertex.  If you can't get it to re-attach, which sometimes happens, just delete the dimension and use the Smart Dimension tool to insert a new one.  Occasionally a dangling dimension will appear to not be selectable (won't turn blue when you click on it), but when that happens I've always been able to click on it anyway and delete it with the Delete key on my keyboard.  I've also run into a situation a time or two when a dimension would turn that color and appear to have lost it's references, but would be all blue when I clicked on it instead of having the red box.  This seems to happen mostly when copying and pasting sheets from one drawing to another.  When that happens I can still click on the box at the end of the extension line and re-attach it.

   While I'm on the subject, notes and balloons (and other annotations) will sometimes lose their reference also and turn that same color.  When that happens just click the end of the leader and re-attach it.

   There's a setting you can choose that will automatically hide these annotations, but I keep it turned off.  If there's a problem with an annotation I want to know about it.  If it just goes "poof" I very likely might not notice.

 

 

   30.  I have a Global Variable (or Custom Property, etc) that I'd like to link to in a Linear Pattern, Distance Mate, or similar feature that contains a dimension.  Is this possible?

   Yes.  Some features, such as Linear Component Patterns in Assemblies, allow the use of Equations directly in the Property Manager (just type the Equal sign in the dimension dialog box, see below), but this was added fairly recently, so may not be available if you're using an earlier version, and still isn't available for all features.

 

   If you can't do it directly in the Property Manager, go ahead and create the feature, using a dimension that's close to what you need.  Click Okay to close the feature, then single-click on it in the tree to show the dimension in the graphics area (or double-click if you don't have Instant 3d turned on).

 

 

   Double-click on it to bring up the standard dimension dialog box, enter the Equal sign, and link to your variable, custom property, etc.  You'll need to do a manual rebuild for the change to take effect.

 

 

   31.  I have an icon in my tree that I don't recognize.  What does it mean?

   Please see this blog post from Jim Wilkinson.  It shows all the icons (or almost all; if you have one you don't see there please let him know), along with links to SW Help for each group.

 

   32.  I'm having problems with a school assignment.  Can someone help please?

  I, or someone else, will be glad to help.  Most of us here enjoy helping others learn more about SolidWorks, and some active forum members are teachers.  If you want help learning then please post your specific question about what part of your assignment you're having trouble with.  Include screenshots of your work at a minimum, and attaching your model will be better.  More and better information will get you more and better answers.

   If, on the other hand, instead of help you want someone to do your work for you, please don't bother asking.  It's dishonest, and you won't learn anything that way.

 

   33.  I have a sketch that was created in my Assembly, and I'd like to move it to one of the Parts in the Assembly.  Can I do that?

   There isn't a way to do that directly, but there are at least two methods that should work for you.  You can copy the sketch from the Assembly and paste it into the Part file, then delete it from the Assembly.  You will need to reapply some relations to fully define it in the Part.  Another option would be to edit the Part within the Assembly, create a new sketch on the same plane as the Assembly sketch (or one that's parallel to it), and use the "Convert Entities" sketch tool to reproduce the sketch entities in the Part.  If you use this option you will of course need to keep the sketch in the Assembly instead of deleting it, unless you first delete the "On Edge" relations.

 

   34.   How do I dimension to the intersection of two edges, such as at a chamfer or fillet?

   With the Smart Dimension tool active, right-click on one of the edges and choose "Find Intersection" from the drop-down.

 

 

Then click on the second edge.  That will insert a Virtual Sharp at the intersection of the two edges, and establish it as the dimension reference.  This right-click option is a fairly recent enhancement (SW2015, maybe?).  If you're using an older version, then exit the Smart Dimension function, Ctrl+select the two edges, and then select the Point sketch tool.  That will place a Virtual Sharp at the intersection of the edges, and now you can dimension to it.  By the way, you can choose which of several styles you prefer for Virtual Sharps at Tools > Options > Document Properties > Virtual Sharps.

 

 

Unfortunately, there isn't currently (as of SW2017) a way to set a Layer or color for them.  You can use a Layer to change the color if you don't like the default.

 

 

   35.   I have an Assembly (or Drawing), and now I want a new one that's very similar.  What's the best way to do that without messing up the original?

With the parent file open, go to File > Pack and Go.  That will allow you to copy the file, and all of its dependent files (Parts, sub-assemblies, etc.) to another location.  Most of the options are self-explanatory, but I'll touch on a couple of them.  If you use Toolbox, there's a box near the top left you can de-select to avoid copying them.  There's also an option near the bottom left to send the files to a Zip file, which is handy if you need to send them to someone (or post them in a forum).

 

Changing the names of the new files is a good policy to make sure you don't get unintended changes to your original files.  There are three ways to do this:

   1.  Double-click on the file name in the "Save to Name" column.  That will allow you to assign a new name to individual files.  This works fine if there aren't too many files, but for those with quite a few use 2 or 3.

   2.  There are checkboxes near the bottom right corner where you can add a suffix or prefix to the new file names.

   3.  Use the "Select / Replace" button (near the center, just below the list of files) to replace text in file names (such as project numbers) with new text.  This function can also be used to exclude some components (such as library parts) by selecting "In Folder" from the Search drop-down, entering a key word, and then selecting "Uncheck item(s)".

 

When you've finished and clicked "Save", be sure to close your original file (I learned this the hard way), then open the new files to make your changes.

 

 

   36.   I have one Part interfering with another one in an Assembly and I want to use the interference to remove material from one of them.  How do I do that?

In the Assembly, click on the one you want to cut and choose the "Edit Part" icon.  That will allow you to edit this Part in the context of the Assembly.

 

 

Now choose the Indent command (Insert > Features > Indent).  Select the Part you want to cut ("Target body:") and the Part you want to cut it with (Tool body region:), and choose "Cut".

 

 

Click on the Okay icon and you're done.

 

 

   37.   When I start a new Assembly there is a Part (or Parts, or a sketch, etc) already there that I don't want.  What happened, and how do I fix it?

Somehow your Assembly Template got saved with the Part in it.  Possibly you (or someone) started a new Assembly, made some changes at Tools > Options > Document Properties, and saved the template after this Part had been inserted.  How it happened doesn't really matter, but it's easy enough to fix.  Start a new Assembly with this template, delete the Part, and then File > Save as > Assembly Template.   Saving it to the same name will override the template with the Part already inserted, or save it to a new name.

By: Glenn Schroeder  Wed, 11 Jan 2017 15:53:29 GMT
Re: FAQ - Part 2

2017-12-12:  I edited #26 and added the part about multiple tabs in the New Document window.

By: Glenn Schroeder  Tue, 12 Dec 2017 17:39:44 GMT
You are not authorized to view this page No results found! Suggestions: Check spelling, try a different search, or browse topics below.