This is something that has annoyed me for quite a while...

dimensions.jpg

 

See all those points? This is the only way I can dimension to mid points, when placing the point on a midpoint, it highlights no problem, but if I try to dimension directly on these midpoints it refuses to acknowledge their existence.

 

Why is this? Am I missing something here? Would really like to avoid having to put sketch points everywhere. Ive put up with this work around for quite some time and I'm really getting sick of this, its such a simple thing that eats into productivity.


Categories: Drawings and Detailing

Comments
Last comment By: Glenn Schroeder   Wed, 14 Feb 2018 20:47:31 GMT
Re: Cant select midpoints to dimension

This probably isn't a much better idea for you, but how about placing some center lines? Or maybe you could show temporary axis' and select them for dimensioning?

By: Jim Steinmeyer  Mon, 12 Feb 2018 22:21:51 GMT
Re: Cant select midpoints to dimension

Hello,

 

You didn't mention it, but have you tried to right-click as you're about to pick and select midpoint from the menu?

 

Cheers,

 

Kevin

By: Kevin Chandler  Mon, 12 Feb 2018 22:25:09 GMT
Re: Cant select midpoints to dimension

Hello Ben... so, even if you use the Selection Filter and choose the select Midpoint option?  (image attached)

midpoint.png

By: Paul Salvador  Mon, 12 Feb 2018 22:40:58 GMT
Re: Cant select midpoints to dimension

Hello,

 

Here's the screen shot of my post above:

 

It's a little extra effort especially if you have many to do or do it often.

I'm in the same boat with sheet metal, having to do this to get an intersection dim (which I submitted an idea on but it didn't do well in the polls).

 

Cheers,

 

Kevin

By: Kevin Chandler  Tue, 13 Feb 2018 13:09:44 GMT
Re: Cant select midpoints to dimension

Unfortunately, "Select Midpoint" doesn't work when selecting edges of cylindrical bodies, such as pipe.  I have the same issue with rebar.  The only solutions I've found are workarounds, and have already been mentioned (sketch geometry, inserting centerlines, or turning on temporary axes to dimension to).

 

By the way, if you do use sketch geometry you can move it into a Layer that's turned off.  The dimensions will still be visible.

By: Glenn Schroeder  Tue, 13 Feb 2018 13:33:15 GMT
Re: Cant select midpoints to dimension

Hello,

 

Thank you for correcting me on this.

I did a test on a round stepped part and "Midpoint" wasn't there.

 

But Intersection was there, so as a test, I added a centerline and the intersection dim does work.

It's another workaround, but as it is with all workarounds, it's added steps for little value added.

 

Cheers,

 

Kevin

By: Kevin Chandler  Tue, 13 Feb 2018 17:19:16 GMT
Re: Cant select midpoints to dimension

add center lines as Jim suggested, or show the sketch that was used to make the pipe.  Really surprised that none ever said where are you centerlines before now.

By: David Matula  Tue, 13 Feb 2018 17:44:09 GMT
Re: Cant select midpoints to dimension

As David and Jim said, I find the easiest way to achieve that is to create centerlines on your pipes. If the pipes are part of the same weldment, then you should be able to just click one face, and it will place all centerlines of the pipe bodies in one go. Sometimes I have awkward difficulty with centerline command, and I end up having to select the cylindrical edges to place it.

 

If you don't wish them to show and obscure your objects, place them on a separate layer, dimension them, then turn the layer off.

 

Depending on how your components are designed (asymetrical or off-center or even just slightly off-center origin helps no one), you can also dimension between component origins. What you can or can't dimension to or from usually depends on what you choose to have visible, and what selection filters are active. I also find that you can select two reference geometries, whether origin, plane, or axis, from the design tree and then start dimension command and place it. But then, I heavily rely on same reference entities in a lightweight assembly because they will carry through in a lightweight component: i.e., my components already have those entities i now refer to.

By: Tom Gagnon  Tue, 13 Feb 2018 17:55:32 GMT
Re: Cant select midpoints to dimension

..sure,..while we are here.. let's also try a midpoint formula!?

midpoint_formula_picture.jpg

By: Paul Salvador  Tue, 13 Feb 2018 17:57:55 GMT
Re: Cant select midpoints to dimension

Paul Salvador wrote:

 

..sure,..while we are here.. let's also try a midpoint formula!?

midpoint_formula_picture.jpg

you're going to make my head hurt, aren't you?

By: Jim Steinmeyer  Tue, 13 Feb 2018 19:15:26 GMT
Re: Cant select midpoints to dimension

To create multiple centerlines w/one click:

select: Create Centerline-> Select Option: Select  View -> Click on the View:

Capture.JPG

By: Vladimir Urazhdin  Tue, 13 Feb 2018 19:21:24 GMT
Re: Cant select midpoints to dimension

Thanks all for the replies.

 

I have tried right clicking, but no midpoint. I could dimension off the sketches I used for the pipe center lines. I tried creating centrelines for the drawing view but it would create a whole lot of lines I don't want. I will use the idea of hiding the points on another layer but no one has complained yet about the points on the drawing view so I will avoid this extra step for now. Also midpoint filter did not work. It appears that that solidworks just doesnt want us to use midpoints when dimensioning.

 

But I guess the point I am raising here is that the midpoint is not available on mouse over (when it should be) like it is when placing a point (or any sketch entity for that matter), if this was the case all the work arounds you have suggested wouldn't be necessary. The work arounds are the productivity hogs that I want to eliminate.

 

I struggle with RSI/ carpal tunnel on a daily basis and Im always looking for ways to reduce the amount of clicking I need to do!

By: Ben Richardson  Tue, 13 Feb 2018 21:26:39 GMT
Re: Cant select midpoints to dimension

Ben Richardson wrote:

 

Thanks all for the replies.

 

I have tried right clicking, but no midpoint. I could dimension off the sketches I used for the pipe center lines. I tried creating centrelines for the drawing view but it would create a whole lot of lines I don't want. I will use the idea of hiding the points on another layer but no one has complained yet about the points on the drawing view so I will avoid this extra step for now. Also midpoint filter did not work. It appears that that solidworks just doesnt want us to use midpoints when dimensioning.

 

But I guess the point I am raising here is that the midpoint is not available on mouse over (when it should be) like it is when placing a point (or any sketch entity for that matter), if this was the case all the work arounds you have suggested wouldn't be necessary. The work arounds are the productivity hogs that I want to eliminate.

 

I struggle with RSI/ carpal tunnel on a daily basis and Im always looking for ways to reduce the amount of clicking I need to do!

 

You can use that feature to selectively place centerlines.  Before activating the feature, make sure you don't have a drawing view (or anything) selected.  Then after activating it, select two edges and it will place a centerline midway between them.  Repeat as needed, then exit the function.

By: Glenn Schroeder  Tue, 13 Feb 2018 21:41:44 GMT
Re: Cant select midpoints to dimension

Hi Glenn,

 

Thanks, but this would be just as much work as the points, maybe even more. The easiest solution I can think of is showing sketches and just dimension off those.

By: Ben Richardson  Tue, 13 Feb 2018 22:29:56 GMT
Re: Cant select midpoints to dimension

adding the centerlines is really easy sometimes it is just a matter of clicking on the pipe. 

it is something that you should play with to see if you want the view to get all the centerlines added or if it would be easier to click on each component that you want centerlines added to....

By: David Matula  Tue, 13 Feb 2018 23:36:21 GMT
Re: Cant select midpoints to dimension

Ben,... I hear ya,.. you have a valid argument as to WHY this does not work well or work BETTER? 

By: Paul Salvador  Wed, 14 Feb 2018 00:19:26 GMT
Re: Cant select midpoints to dimension

Hello,

 

Another thought: Do you have access to your fiiting models?

 

If so, how about adding a little cut (or something) that adds a line segment at the middle of the silhouette edge?

 

This way you will always have a line edge to dim to directly.

 

Each fitting would need to be modified on all quadrants for each end, nut once done, it is normal one click dimming from then on.

 

Perhaps a split line along the axis at the connection instead of the cut, but something that allows for minimal clicks to add the dim.

 

Cheers,

 

Kevin

By: Kevin Chandler  Wed, 14 Feb 2018 04:04:51 GMT
Re: Cant select midpoints to dimension

Hi, Ben

You can use part (assembly) annotation tool. It is like creation of your drawing views but in part (assembly) file.

You will have access to the whole geometry and it takes a few seconds to import these annotations to the drawing views.

It saves a lot of time in case of drawing recreation too.

By: Igor Fomenko  Wed, 14 Feb 2018 05:26:22 GMT
Re: Cant select midpoints to dimension

Ben Richardson wrote:

 

Hi Glenn,

 

Thanks, but this would be just as much work as the points, maybe even more. The easiest solution I can think of is showing sketches and just dimension off those.

 

That should work fine.  By the way, you probably already know this, but after placing the dimensions if you hide the sketches so they don't show the dimensions will also be hidden by default, but you can right-click on the sketch in the tree and choose "Show Dimensions" (I'm at home right now and don't have SW here, but I believe that's the correct terminology).

 

Just thought I'd mention that in case someone might not want the sketches to show after placing the dimensions.  I learned about it not long ago from Deepak Gupta.

By: Glenn Schroeder  Wed, 14 Feb 2018 20:47:31 GMT
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