CAD Forum

. . . and it's not even Christmas. I'm working in a Drawing and placed two dimensions referencing a point in a model sketch, then hid the sketch, like I've done hundreds of times. BOTH DIMENSIONS REMAINED VISIBLE.

I don't believe that's ever happened before. Usually one of the two dimensions will also be hidden, and occasionally both, so that I have to scroll down to the sketch in the tree, right-click on it, and select "Show dimensions" from the drop-down.

Version?

Interesting. Yeah, I wonder if it's the points you used or if there's a new Hide/Show option available to display the orphaned dims?

I'm using SW2023, but I've been using since it was first released, and I do this type of drawing in a weekly basis and I don't remember this happening before. It is no exaggeration to say I was astonished when I hid the sketch and both dimensions remained visible.

Hidden in one display state, drawing view using a different config/display state?

There is an option to show the dimensions.
It's not new....I see it in 2019.

Glenn Schroeder wrote: ↑Fri Mar 24, 2023 2:19 pm . . . and it's not even Christmas. I'm working in a Drawing and placed two dimensions referencing a point in a model sketch, then hid the sketch, like I've done hundreds of times. BOTH DIMENSIONS REMAINED VISIBLE.

I don't believe that's ever happened before. Usually one of the two dimensions will also be hidden, and occasionally both, so that I have to scroll down to the sketch in the tree, right-click on it, and select "Show dimensions" from the drop-down.

I have to confess in all my years of workign in SW, I've never made Drawing dimensions that reference sketch elements in a Part. Huh.

I use them to create prints like this for the marketing department. It is the only way I can get it to measure the right things on the correct plane.


I know solidworks can't read my mind, but the whole point of those sketches is for the dimensions I create. Why would I want those dimensions hidden when I hide the skecth?

jcapriotti wrote: ↑Fri Mar 24, 2023 6:18 pm There is an option to show the dimensions.
It's not new....I see it in 2019.

The problem is that when you hide the sketch, the dimensions get hidden with them, so you have to use the option you show to turn them back on.

Rather than create a sketch, you can create a small circular planar surface in the model. It won't show up in the drawing, but it will prevent the dimensions from disappearing when you hide the sketch. As an added bonus, you can hatch the surface to make it look like an actual point:

JSculley wrote: ↑Mon Mar 27, 2023 8:06 am Rather than create a sketch, you can create a small circular planar surface in the model. It won't show up in the drawing, but it will prevent the dimensions from disappearing when you hide the sketch. As an added bonus, you can hatch the surface to make it look like an actual point:

image.png

Unless the part goes to an assembly that has a drawing in which you do not want to see the surface.

bnemec wrote: ↑Mon Mar 27, 2023 10:17 am Unless the part goes to an assembly that has a drawing in which you do not want to see the surface.

A display state solves that problem.

JSculley wrote: ↑Mon Mar 27, 2023 11:46 am A display state solves is a workaround to that problem bug.

FIFY

bnemec wrote: ↑Mon Mar 27, 2023 11:57 amFIFY

Fair enough. SW considers it to be working as designed (S-053776). Surfaces are considered reference geometry in parts but are considered bodies in assemblies.

There's an SPR (725625) requesting consistency between the two document types.

SW also exports the surface if you export an STL, which made for some very strange prints before I figured out what was going on.

m2shell wrote: ↑Sat Mar 25, 2023 10:27 am I have to confess in all my years of workign in SW, I've never made Drawing dimensions that reference sketch elements in a Part. Huh.

I only do it for one specific purpose. Here where I work we do vehicle crash tests. The test report needs a drawing showing the test vehicle approaching the impact, leaving the impact, and the final resting place, with dimensions referencing the final resting place. I use an Assembly sketch to mate the vehicles in the correct locations, and since the sketch is already there I use it for the dimensions. If I didn't do that I'd have to add sketch geometry in the Drawing (which I would then need to hide).