Modelling part in different positions

[Pierrec]

Hello everybody,

I'm rather new to SW (coming from AutoCAD), and I'm not too sure what the right approach is to what I'm trying to do. Here's my problem:

I have an assembly with two parts: a main part (let's call it A) with a hole in it and two pegs on each side, and a level-like part (I'll call B) with a cylinder that rotates inside the hole, and an "arm" that can move from one peg to the other.

The pegs act as stops for the arm on part B, so that B can only rotate +-25 degrees on each side. The problem is that these pegs have rather convoluted shapes, and the arm on part B must has similar shapes on both side, in negative, so that when it rests on either peg, the peg "disappears" into the arm. These are parts that, in real-life, are made and adjusted by hand, and I need to model them.

So what I wanted to do is this: I started by modelling the arm of part B with an oversize square block, then I assembled B onto A with the proper mates, and then (this is the bit I can't figure out), I would like to move the lever to its proper position on the right peg, use the right peg to imprint its shape into the right-side of the arm, then move the lever to the left and do the same with the left peg, so that in the end, I have my lever arm with both sides imprinted with the shape of both pegs.

How to I go about doing this? I've tried doing this in various ways, but it doesn't work at all and I have a feeling I'm not using the right approach at all, so I'd be glad if someone could point me to the right direction.

Come to think of it, I'd also need to position another part in different positions to pick up external references in the part's sketches with the part in one position, and other external references with the part in another position: is this the same problem?

I'd be extremely grateful for any help you can provide with this. Thank you very much!

EDIT: I forgot to mention I use SW 2008


Edited by: Pierrec

 

[ProE_Addict]

If I understand your problem correctly, it sounds like you're on the right track.


Create the negative contour on B by converting the contour from the pin in A. After converting the edge, delete the references it has to pin in A. This keeps the profile, but will no longer be a parametric link. Then create your cut/boss feature.


Rotate the pin the other direction and repeat.


If you need to change the contour later, you'll have to recreate the profile by again converting the edge and deleting the relations.

 

[jimshaw]

Agreed - The key is to remove the relations after converting the lines, so that when the parts move in the assembly, the references DON'T update.


If you use a mate angle you should be able to control how much "imprint" the pegs have onto the arm.


Hope this helps.

 

[Pierrec]

Create the negative contour on B by converting the contour from the pin in A. After converting the edge, delete the references it has to pin in A. This keeps the profile, but will no longer be a parametric link. Then create your cut/boss feature.


Rotate the pin the other direction and repeat.


If you need to change the contour later, you'll have to recreate the profile by again converting the edge and deleting the relations.

Ah, it works, but I was rather hoping I could make this fully parametric. In reality, I over-simplified the description of the problem to avoid confusing the issue. What happens is, the lever's excursion depends on the exact shape of the pegs, which itself depends on the position of other parts, so I wanted to maintain a dependency between the pegs and the lever. Other parts depend on the lever's range of motion also, so I don't want to manually edit the thing each time I make a change.

Ideally, I would have liked to be able to be able to go edit the lever part, and insert a function such as "Position part in assy", with a scope limited to the part editing, or perhaps have whatever function I want to use at the time (boss, sketch, whatever) be tied to a temporary configuration of the assy. This doesn't seem to exist however.

I think I found a workaround for my problem: I insert part A (the one with the pegs) in part B as a volume, position it with mates so that the lever ends up on the left side where it should be, "imprint" the peg, then rotate A so that the lever is on the right side, and do the same, then I remove the volume I inserted. That seems to maintain relationships fully between A and B, but it seems like a heavy solution to the problem. The other drawback is, for some reason, when I go back into the assy with the lever "imprinted" on both sides that way, I can't seem to be able to use collision detection when I position the lever. That might be because the contact surfaces between the imprints in B and the pegs on A are too complex however, I'm not good enough to know why yet I'm afraid.


Anyway, thanks to both of you for your answers, I really appreciate it!

 

[Mihail]

Insert two more parts (the same arm), mate this arms one each side and use them to define the necesray sketches (with CONVERT ENTITIES) and DO NOT remove the references. After that hide this phantom arms. It is an idea but I do not try that. Sorry for my english, hope you unterstand.

 

[Rimma]

In sach case i do so way


1. create some features you needed forpart Binside your assambly(1) with references.


2. create new assambly (2) with different name and insert your parts with matches. By so way you save references and nesessary moving.