Parts in assemblies

[prooney]

I have a little dilemna/question and I hope I'm not making more of this then I need to. I have this assembly which is made up of two separate parts the first part we'll call "A" is a piece of flat plate that gets machined.

Part "B" is a piece of round bar that gets welded into part "A" to make an assembly. At this point the assembly then gets machined to the final part.

Here's my dilemna, what's the best way to draw part "B" so that I only have one part file for this piece of round bar. Would it be to draw the part completed and then suppress it to it's initial state after it's cut to length? Then show the final machined piece in the assembly?

I hope I didn't confuse anyone with my explanation. Thanks in advance.

 

[CorBlimeyLimey]

Create the assy with the non-finished parts and then use the Insert > Assembly Feature > Cut > Extrude option to create the machined assy. The assy components will not be affected at the part level.

 

[prooney]

CorBlimeyLimey,

Thanks for the reply, what if the part has multiple features such as a thru hole, a side hole going into the thru hole and an internal hex on one end? Would this be able to be all done during the assembly stage and still not affect it at the part level?

 

[handleman]

It's also possible to insert a part into another part, and even position it using "mates". If you're going to do much machining after welding and you don't need to have a BOM for the weldment you might want to check into that functionality.

-handleman, CSWP (The new, easy test)

 

[prooney]

Insert a part into a part? Could you explain further handleman?

The assembled part is going to get the thru hole, side hole, OD and hex machined into it after welding.

 

[CorBlimeyLimey]

Any features created by the Insert > Assembly Feature > Cut > Extrude option are not propagated to the part level.

 

[handleman]

Insert a part into a part is just that. If you have a part file open (either an empty file or one that has geometry/features already) you can click Insert->Part and choose any external part file to be inserted into your current part. I guess I forgot to mention that mating is only available in 2007 (I think) or later. When you insert a part into another part, the geometry (without features) is inserted into the new part as a solid body that is linked back to the original part you inserted. If you change the model of the part you inserted, the "composite" part will update with those changes. However, changes you make in the "composite" part won't propagate back into the inserted part. You can perform any actions you want in the "composite" part - cut, extrude, sweep, fillet, whatever. Assembly features are limited to material removal only. You can't add material using an assembly feature. Some limitations of inserting a part into another part are limited mates available and no BOM for the "composite" part.

-handleman, CSWP (The new, easy test)

 

[grunt58]

Handleman,

Is there a way to break that x ref or keep the original part from opening in the background? I've inserted a part into a part but not when I open the "composite" part it opens the original part in the back ground.

sorry this probably should have been a new thread.....

Thanks

Grant
Applications Engineer
SW2008 X64 SP 3.1
Dell Precision T5400
Nvidia Quadro FX 5600
Xeon 2.5GHz Quad Core, 4GB RAM
XP Pro X64 SP2.0

 

[CorBlimeyLimey]

grunt58,

Go to Tools > Options > System Options > External References and set the Load referenced documents option to None.

 

[gwubs]

prooney,
Go with CBL's method. At our company, we find that the best way to set up parts and assemblies is to emulate what actually happens. In your case you will be able to draw the parts to be cut, detail how they are assembled and then machined, within the assembly. Sometimes people argue against going this route because it seems to be more work, but in the end, it pay off big time because you can just hand off drawings without explaining that something detailed on a part drawing actually needs to happen in an assembly & etc. It also promotes the ability to reuse parts and assemblies, with their accompanying drawings in future.
We have used this method for 5+ years, and believe me it is worth doing. Good luck.
Gerald

 

[prooney]

Gerald,

I followed CBL's suggestion and as you stated it does seem to be the best way. It makes more sense to me to do it this way.