Machining of a weldment assy

[EricLeBlanc]

Hi there,

I have created an assembly of parts that needs to be welded together . Than, I have to machined the welded assy. What would be the proper technique to be able to produce a welded assembly and a part refering to the welded assy who would become the "as machined". Of course the part needs update if the assembly change...

I have played around with Merge, Inheritance, Copy Geom...but all those command works well with a part but not with an assembly.

I have tried Edit - Component Operations - Merge. With that I can produce a merge part from an assembly but part does not update if I make changes to the assembly...

I'm new to PRO/E, I'm use to Catia where I can use the command "associate part" to do what I'm trying to do...

Thanks for helping!

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[DavidButz]

4 comments:

(1) If you are concerned about machining using Pro/NC, you can machine assemblies as well as parts, so you don't necessarily have to create a separate part.

(2) Similarly, you can add remove-material features (cuts and holes) to the assembly, and choose whether or not they appear at the level of the part.

(3) When you do a Merge operation, you have a choice between Reference and Copy; if you pick Reference, changes to the parts of the assembly should be seen in the Merge part.

(4) If you use the Merge method, a good method is to assemble an empty (no solid geometry) part into your assembly, and merge all the other parts into it.

[nico74]

If you go for the option 2, removing material feature in the assembly. There are a few limitation.

You cannot add any radius you need to integrate them in your sketch. and I think the hole tool as some limitation too.

[DavidButz]

Nicolas,

I'm not sure I know what you are referring to with respect to either adding a radius or limitations of holes. Certainly, you are limited with what solid features you can add in an assembly. If you think about it, the reason is simple. The Assembly is really just a set of instructions for locating Parts; the Parts contain all the solid geometry. Thus, it's possible to "carve away" within the assembly, but there's no place for add-material features to reside within the Assembly itself.

If by "radius" you are referring to adding a round (maybe a fillet to represent a welding bead?), that is not possible because of the add-material restriction. If you really want that functionality, I would recommend going the Merge route.

David

[nico74]

Hi David,

By adding Radius I was thinking of adding a radius on a cut made in the assembly.

I know you can add the radius in the sketch but it's sometime easier to add it afterwards. (Making a cut with a ball ended cutter in an assembly is pretty difficult)

Technically you only remove part of the carve made before you don't add material.

Nicolas

PS does the merge route keep different hatching at the drawing level?

[DavidButz]

Hi Nicolas,

1. If you Merge, you will not preserve the hatching, because you are going to end up with one part.

2. For your ball mill cutting example, another thing you might look at is creating a Surface in the Assembly, which can be copied into whichever Parts it affects, then used to remove material from those Parts. (I don't know if that will be useful in your particular case or not.)

David

[GregMerz]

Hi Eric,

Did you ever resolve this and how? I am doing the same thing. I also read all the replies.

Thanks

[nico74]

Hi Eric,

I wouldn't go thru the merge route myself. Has I prefer to keep different hatch for different part.

Then depending on how you detail your welding part would choose different line.

1. If You only want an assembly drawing with all dimension for manufacturing I would add the difficult cut in the part level.
   The hole thru tool is also a pain in assembly mode so I would add the hole in the part. But if the hole is the use in a pattern in different part then you have to use it in the assembly.
   For the ball nose cutter cut I was referring before you can make it with multiple operation in the assembly mode (extrude cut and revolve cut) but it's much easier in the part mode with the extrude tool and fillet tool.
2. If you want to make drawing of all the part before the weld process but don't think the hatch is an issue you can use the merge route (i can't comment as I've personally never used it)
3. If you want to have part drawing and the hatch I beleive the only option is to make the cut in the assy mode.
   A nice trick I've read on a forum was for the thru hole. when you want it thru one part only make it from the inside to the out side. (you can not do hole to surface or to next in assy mode)

I hope this is usefull. I wish you good luck keep adding more trick and tip as you go along.

Nicolas

[EricLeBlanc]

Thanks to all for your imput!

Here's how I end up doing what I was looking for:

1. Make your welded assy as per usual

2. Create a new component in assembly mode. I choose "empty" in the Creation Method menu

3. activate the new component.

4. Insert - Shrinkwarp - in the right scroll down menu choose Autocollect All Solid Surface.

5. Click the Option tab and check Solidify Resulting Geometry. Also check Leave As Quilt Solidification Fails. Accept the command.

6. Save your ass'y and the "new component" This component will be used as a transitionnal part...

7. Start a new part. This part will become the machining part.

8. Insert - Shrinkwrap - Open the "transitionnal part"

9. Placement - Default.

10. Click Reference tab. Click the upper box Always Include Surfaces. A small window will open with the shrinkwrap model.

11. Click on one surface on the shrinkwrap model.

12. Right click and choose Solid Surfaces. Accept the command.

13. In the model tree, click the + before External Shrinkwrap id

14. Select Ext Ref Copy Geom id

15. Edit - Solidify. Accept the command.

16. Voilà!

With this method, if you do modifications on the weldment ass'y they will appear in the machined part. One downside is that you have one single hatch pattern for the machined part but I never found this to be a problem so far...

Eric