part sketch driven .SLDDRW lines not updating

[Mike Gera]

I occasionally use .SLDDRW lines that are driven by a part sketch. Please see attached example.

Note that the notch in the lower-left corner is out of sync with the driving part sketch.

What causes this, and how is it corrected?

Thanks.

[JSculley]

You have two over-constrained sketch relations in your drawing sketch:

They are preventing the sketch from updating correctly

[Mike Gera]

You have two over-constrained sketch relations in your drawing sketch:

image.png

They are preventing the sketch from updating correctly

Thanks!

This (type of) problem has been bugging me for literally months.

I wonder why I wasn't seeing an error message.

[Glenn Schroeder]

Thanks!

This (type of) problem has been bugging me for literally months.

I wonder why I wasn't seeing an error message.

If you will set relations to show when you're working with an active sketch then ones with problems will be red or yellow instead of green, which will indicate a problem.

[Mike Gera]

If you will set relations to show when you're working with an active sketch then ones with problems will be red or yellow instead of green, which will indicate a problem.

Hey Glenn, thanks.

Specifically, what setting would that be?

[SPerman]

https://help.solidworks.com/2021/englis ... le_Display

How do I toggle the display of sketch relations?
Click View Sketch Relations (View toolbar) or View > Hide/Show > Sketch Relations to toggle the display of sketch relations. If you clear View > Hide/Show > Sketch Relations , but you select a sketch entity in an open sketch, the sketch relation icons appear.

[JSculley]

https://help.solidworks.com/2021/englis ... le_Display

How do I toggle the display of sketch relations?
Click View Sketch Relations (View toolbar) or View > Hide/Show > Sketch Relations to toggle the display of sketch relations. If you clear View > Hide/Show > Sketch Relations , but you select a sketch entity in an open sketch, the sketch relation icons appear.

In a drawing, you have to go a step further. The only way to see the relations is to click on a sketch element on the drawing or the sketch feature of the model in the feature tree.

[Mike Gera]

In a drawing, you have to go a step further. The only way to see the relations is to click on a sketch element on the drawing or the sketch feature of the model in the feature tree.

I noticed that as well. Thanks.

Is there a setting that will throw an error when over-definition occurs in an .SLDDRW?

[Glenn Schroeder]

I noticed that as well. Thanks.

Is there a setting that will throw an error when over-definition occurs in an .SLDDRW?

You should get one or more notifications near the bottom of your monitor on the status bar.

[JSculley]

I noticed that as well. Thanks.

Is there a setting that will throw an error when over-definition occurs in an .SLDDRW?

Nope. You either have to select the sketch or the view to see any errors.

Have you considered an alternate approach? You can create a planar surface from your sketch in the model:

and then you don't need to convert entities at all in the drawing:

image.png (5.13 KiB) Viewed 1082 times

[Mike Gera]

Nope. You either have to select the sketch or the view to see any errors.

Have you considered an alternate approach? You can create a planar surface from your sketch in the model:

image.png

and then you don't need to convert entities at all in the drawing:
image.png

Thanks for the suggestion. Sounds interesting. I've never done anything with surfacing. How would I go about it?

[JSculley]

Thanks for the suggestion. Sounds interesting. I've never done anything with surfacing. How would I go about it?

Create your sketch:

Then Insert...Surface...Planar (or use the command from the Surfaces toolbar):

image.png (28.73 KiB) Viewed 1046 times

[Mike Gera]

Create your sketch:

image.png

Then Insert...Surface...Planar (or use the command from the Surfaces toolbar):
image.png


image.png

That's probably better than what I'm currently doing, but I think I'd still have the same problem when it comes to construction lines.

[JSculley]

That's probably better than what I'm currently doing, but I think I'd still have the same problem when it comes to construction lines.

Possibly. You should strive to eliminate sketch entities on drawings if at all possible. Perhaps if you could provide some detail on what you are trying to do that led you to this workflow, people will have ideas on a more robust and possibly better method.

[Glenn Schroeder]

Possibly. You should strive to eliminate sketch entities on drawings if at all possible. Perhaps if you could provide some detail on what you are trying to do that led you to this workflow, people will have ideas on a more robust and possibly better method.

I agree. Even if you don't want to create a surface or solid body with the model sketch (though you usually should), doing the sketch in a model and inserting a drawing view of it in the Drawing is almost always a better choice than sketching directly in the Drawing.

[Mike Gera]

I agree. Even if you don't want to create a surface or solid body with the model sketch (though you usually should), doing the sketch in a model and inserting a drawing view of it in the Drawing is almost always a better choice than sketching directly in the Drawing.

I'm using SolidWorks to create an architectural floor plan.

Do I have AutoCAD? Yes. Could I use it? Yes.

I prefer the parametric, relation-driven sketching in SW, though, so I'm trying to make it work.

[Glenn Schroeder]

I'm using SolidWorks to create an architectural floor plan.

Do I have AutoCAD? Yes. Could I use it? Yes.

I prefer the parametric, relation-driven sketching in SW, though, so I'm trying to make it work.

I haven't done architectural plans, but I did once do a drawing of our offices to make a layout with the names, phone numbers, office numbers, etc. I still did it in a model, then imported that into the Drawing.

[Mike Gera]

I haven't done architectural plans, but I did once do a drawing of our offices to make a layout with the names, phone numbers, office numbers, etc. I still did it in a model, then imported that into the Drawing.

Glenn,

How exactly did you do that, if I may ask.

Thanks.

[SPerman]

I did it as an assembly. Everything is a solid. This is the same process I use for everything I model. I didn't see a need to reinvent the wheel to create the plan view of our shop.

[Glenn Schroeder]

Glenn,

How exactly did you do that, if I may ask.

Thanks.

Just like @SPerman described above. In my case the walls were all a single Part file, but not a single sketch. I dislike complex sketches for several reasons.

[jcapriotti]

Just like @SPerman described above. In my case the walls were all a single Part file, but not a single sketch. I dislike complex sketches for several reasons.

Too many relations complicated the relationship....applies to CAD tools as well