Assembly Sketches & Features?

[leeave96]

Assembly Sketches & Features?

Is it possible to create an assembly of several parts and then from the assembly, sketch a hole on one of the parts and then extrude it through the assembly?

Further, if this is possible, can you then drive the new hole BACK to the original parts?

I'm trying to create an assembly of sheet metal parts and would like to apply the holes AFTER the assembly where I can apply the holes for fasteners in the context of the assembly vs at the piece part level.

Thanks!
Bill

 

[moyesboy]

You can open each part in the context, and reference geometry from the other assembly parts. but there is no automatic associative link between the parts if you change the hole positions in one of them.

 

[Willbur]

As far as I know, there's no way to extrude through the assembly as a whole, but you can extrude through each part individually and associate the holes. Basically the procedure is the following:
1. Open the assembly (assuming that you've assembled the parts already).
2. Pick one of the parts with a hole in it (generally the easiest of the set to dimension the hole - you will only dimension it on this part) in Design Explorer, right-click and hit Edit Part/Subassembly.
3. Create the hole in this part using either extrude cut or the hole command.
4. Pick the next part in design explorer, right click and hit Edit Part/Subassembly.
5. Create a hole in this part. You have 2 options at this point - if you just want the location to update and the diameter to be fixed, you can use the hole command and apply a concentric constraint between the node and the hole in the other part; otherwise use the extrude cut, draw a circle, and use coincident curve constraint to match both center and radius (this is the one that shows a circle and an equal sign).
6. Repeat 4&5 for other parts.

At this point, anytime you move the hole in the first part the others will update on a regeneration (or 2) of the model in the assembly workspace. When you save the assembly, the holes will appear in each of the parts when you open them separately - if you change the original hole dimensions in the part workspace instead of the assembly, you will need to reopen the assembly to update the locations in the other parts.

 

[Gaspar]

You can create the hole in one part (in part context) and then, within the assembly, edit the next part. Create a sketch and proyect the edge of the hole from the first part into your sketch. Be sure to check the "mantain associativity" box. Use the projected geometry to extrude the hole on the second part and repeat the process with every other part.

This way, if you move or modify the first hole (in the first par) it will be updated automatically in every other part.

Hope this helps!

 

[Gaspar]

Willbur,

Sorry about the double post. Your post wasn't there when I started writing mine :wink:

 

[Willbur]

It's interesting that we were both writing the same thing at just about the same time... :lol: