Yesterday and today I ran into some problems when I updated an assembly and it dealt with how we create our assembly drawings. The way that we make a drawing of our assemblies is outlined in the steps below.
- Create a new configuration of the assembly
- Make an assembly level cut that will give us our desired drawing view
- Make a drawing of the sectioned assembly configuration
For the most part this process has worked well for us in the past but we run into some problems occasionally when we modify an existing assembly. When you add features (that are in the portion of the assembly that is being cut away for the section configuration), SolidWorks seems to have a hard time with any relations that may have been added. For example, I have an existing design that has 2 plates that are bolted together. Down the road I decide that I really need to bolt the 2 plates together in 1 more place. So I edit the components, add a counterbore in 1 of the plates and a tap in the other with a relation that is keeping the 2 features tied together. Are you following me? Here is where the problem happens. These features are in the portion of the assembly that is being cut away for my sectioned configuration and drawing. When I switch to my sectioned configuration I now have an error in the plate that has the relation in it for the counterbore and tap that I added. Now, I noticed that you only get these errors IF you added features after the assembly cut has been created. So now what? I can either delete my assembly cuts, which MAY result in me having to redo a portion of my drawing that is already created or I can run into my computer with a forklift and not have to worry about it for a little while.
Well, I think I may have found a fix today after playing around with it for a little while. Below you will see an image of my 2 configurations that I am working with.
These 2 configurations have already been created and a drawing has been made of the section view. The best that I can tell, in order to have your assembly work OK with features that are added after you have your assembly cut done already you need to roll your ASSEMBLY FeatureManager bar up above the assembly level cuts for your section view. I show a before and after image of your FeatureManager bar below so you can have an idea what I am talking about.
BEFORE
AFTER
Once your bar is rolled back as shown in the “AFTER” image above you can edit your assembly and it will react to your edits correctly.
How do you make sectioned views for your parts or assemblies for your drawings? I do realize that you can create section views in drawings but I do not want to have a view in my drawing that I am not going to print, and I only want to print the section view. If you have other ways of doing this that have worked well for you please share.
I hope this helps anyone that has struggled with this in the past.
Jason,
I’m not sure, but I think that according to ASME specs (Y14.3, sec. 3.1.2), you need to have a defined view to pull a section view from… If you’re not using the specs for your drawings, shouldn’t be an issue.
To get the view you are after (without using a parent view), I would just place the view in the orientation you want and then do a Broken-out Section view.
Brian
http://www.cadfanatic.com/
sorry it took me so long to reply back to you Brian. it got crazy over here at the end of last week.
we do not really conform or callout a sort of specs for our drawings so it leaves us wide open. all of these drawings are for internal use only.
i did play around with the broken-out section a little but I was concerned with how it would react during a design change. when you create sketch for a broken out section what surface does it get created on and what happens if the surface gets modified. too many uncertainties for me to be comfortable.
thanks for the comment and suggestions.
You can specify a depth instead of choosing a specific face or edge to cut to. The surface the broken-out section view is created on and dimensioned from is the closest face/edge in the respective view.
The only thing that I see that would cause an issue is if you add something to the model that would cause the closest face/edge to become “closer” to you; i.e., expands the model envelope out of the paper in the respective view. Even then, it shouldn’t be a biggie…
Create the broken out section to it ends at a custom plane and have that plane based on a location on the part or assembly. That way if the geometry changes thickness, the broken out section will always end at that plane…