Updating Weldment Profiles

[ecarr]

We have several custom weldment profiles we use which we have to update frequently. The problem is the weldments that reference these profiles (.sldlfp files) do not update automatically. The only way to update the parts that I have found is to change the weldment profile (called 'Size:' in SW) and then re-select the original profile. There has to be another way!

Does anyone have any thoughts about what I could be doing wrong?

 

[brengine]

No way that I know of. I do the same process you described to update my Structural Members. When you insert the Structural Member, you are actually copying the Weldment Profile (at that point in time)...no link will remain between them (as you found out).

Ken

 

[CorBlimeyLimey]

You are not doing anything wrong ... that's just the way it is.

However, there is another way. You can edit the profile directly in the sketch of the Structural Member in the FM tree ... just like you would edit a regular features sketch.


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How to get answers to your SW questions FAQ559-1091

 

[ecarr]

Thanks for your replies. After some more searching I found a thread that describes another method that updates very nicely.

Option 2:
Another method to accomplish the desired result is to create the master sketch and create an extrusion. Save the extrusion as a part file. Create a new part file, go to Insert > Part and select the extrusion. Insert a sketch on a plane that sections the profile of the extrusion, select the face of the sectioned extrusion and convert entities. Close the new sketch and delete the extrusion body from the newly created part file. The result is a sketch that is parametrically linked to the base part, so when the base part or "master sketch" is updated the resulting part files will also update.