Assembly Cut

How do you make an assembly cut?

I have two parts in one assembly that I need to line the holes up to be screwed in together. I'd like to make an assembly cut thru the pieces so the holes line up.



Thanks

Todd

What release are you using? In Wildfire you just create a cut as you would in a part, the only difference being that you can choose which parts the cut intersects. I seem to remember it being the same in previous releases.

Yeah, it wasn't really hard at all. Just thought it might be a little more complicated than it was.

Thanks

But just for kicks, is there a way to make the assembly cut show up in the parts individually?

Don't know why you would want to put the cuts in at the assembly level. Your parts become tied to the assembly. Every time you would check out the part/drawing, you would need the assembly because of the cuts. I would put the holes in one of the parts and use ref dims in the assembly to figure out where I needed to put the holes in the other part. Or you can modify one of the parts in the assembly and add the feature at the assembly level. You would have to ensure you have no references to a part in the assembly or the assembly.

In 2001 you get a menu that specifies level after finishing the sketch, which asks which parts get intersected and at what level you want the holes to show up at. The default is Top Level and you would change this to Part Level.

>Don't know why you would want to put the cuts in at the >assembly level. Your parts become tied to the assembly. >every time you would check out the part/drawing, you would >need the assembly because of the cuts. I would put the holes >in one of the parts and use ref dims in the assembly to figure >out where I needed to put the holes in the other part.



This seems absurd to me (no offense donha, it probably isn't to others). I do 95% of my cuts in the assembly level. If you are bolting 3 plates together, is it more efficient to make one cut or 3 (plus having to make ref dims)? In fact I don't even have to sketch a hole or spec c'bores or anything. All my cut data comes from the components that the cuts are for. I just pick a quilt and solidify. If a change the bolt or its location, all the related cuts and locations change automatically. Having to open the assembly to make a change is no big deal (its usually open anyway).



Something goofy about wildfire (that donha mentioned) is the auto-intersect components is on by default and it selects all these components you don't really want it to. It is really annoying. Does anyone use the stupid option? And the default to Top Level cuts means they don't show up in at the part level. Does anyone use this? Why would you ever want a cut to show up in just an assembly? It is not deliverable to anything except an assembly view on apiece of paper!



This means that in WF if you want your cuts to show at the part level you have to ncheck the auto intersect option, highlight all the interseceted components in the list, right-click-remove, set level to part level, and pick your intersected components...Now that's a real improvement. What a waste of time!



I think about half of WF's changes need to be reverted back to 2001.

rcamp,



This means that in WF if you want your cuts to show at the part level you have to ncheck the auto intersect option, highlight all the interseceted components in the list, right-click-remove, set level to part level, and pick your intersected components...Now that's a real improvement. What a waste of time!

I was about to post this problm in WF. You are absolutely right.



Israr

So, Israr, you don't use the autointersect option either?



What about Top Level intersections?



Did you know they cause invisible instances? I had a guy who wasn't setting his assembly cuts to part level, and then whenever an assembly cut failed, after you resolved it, it would fail again as an instance! It would list the part as instance of #F01 or something strange. It took a while to figure out what he was doing to cause this, because of another long-standing ProE quirk: when you redefine an intersection, it always shows Top Level even if it was defined as, and is, a Part Level cut. All the while he was leaving the INtersection set to Top Level.

Once I learned about intersecting parts, all was well. donha, I agree w/ rcamp that it is much easier if you have a complex assembly to make the cut once and then intersect the parts on the assembly to show up on the detail level. But there's got to be some good reason that you'd want your cuts to show up in your assemlby only. I admit, I have no idea what that would be though.

Long ago, when I was a support person for Pro/E, I had a client that was having a similar problem, but he just wanted the cut to show up in the assembly only.



The reason was the parts were recieved from their vendor in tact and the cut (a drilled hole in this case) was added during their assembly process.



Just in case you were wondering why this is an option...

>The reason was the parts were recieved from their vendor in >tact and the cut (a drilled hole in this case) was added during >their assembly process



Then it seems more logical to have the assembly cut intersect at the part level and create an assembly instance with and an instance without it.



eg:



PREPROCESS (instance without the cut)



and



POSTPROCESS (instance with the cut).

I guess we all have our own reasons for doing things certain ways. The company I work for frowns upon external references. There are many of us working in the same areas at the same time. I am just wondering if you do component drawings of the seperate components, and you needed to change only one of the parts to meet FPA requirements, how you would accomplish this when one assembly level feature controlled more than one part?



In days past, there was only one way to create post-part features and that was through assembly level features. With the advent of inheritence features, we now have two ways to accomplish the objective.