Projecting a reference in assembly mode

[v_shankar1979]

Hi there,

I am using ProE Wildfire.

I am creating component in assembly mode. I am trying to project a hole/profile from one part to another part as I need the cut/extrusion of same profile/dimension. Is there a way to do that in ProE?

Thanks in advance,

Shankar.

 

[Israr]

can you attach portion of your assembly and what you want or an image of that? Your question is very clear. Reply to your question is yes, what I understand, there is a way. When you enter the sketcher make use of the use edge command .

Anyhow may be this not what you want. So elaborate your question a bit more.



Israr

 

[v_shankar1979]

Hello Israr,

Here is what I want.



I have assembled 2 components and I have made one component active so that I can modify it. I want to fasten the 2 components together. For that I want to create a set of holes in the inactive part over the active part. When I try to choose a reference to create holes I have no clue how to proceed further to draw datum curve for cut protrusion. Hope the question is clear for you this time.

Thanks,

Shankar.

 

[jabbadeus]

You're talking about creating features using external references. This is a very common procedure and easily doable.



The thing is, you want to do it correctly using proper design techniques.



The best way is to create a Copy Geom feature in the target part (what you call the active part) that copies the relevant geometry (e.g., axes or surfaces) from the source part.



Select the target component in the model tree, right mouse click and hold, and select Insert Feature. You want a Data Sharing (or Shared Data feature, depending on the menu) of the type Copy Geom. Underneath Misc Refs in the dialog box, you can select Axes.



Then when you open the target part, you'll have the necessary geometry so the holes line up. And it's all parametric (source changes, then the taget will change) unless you turn off change propagation by toggling the Dependency option in the Copy Geom model dialog box.



That's the medium-length answer without going into a whole lot of details and particulars.



Dave

 

[donha]

2001 way: Modify>Modify Part> Choose your part you are wanting to put a hole in >Feature>Create>Slot Select your sketching plane, sketch the feature as close to the existing hole in the other part. After creating your hole, Setup>Ref Dim and create a vertical and horizontal Reference Dim. Change the dimensions on your new hole to match the hole on the other part. If you choose this route, you will not create any external references, which are basically a no-no unless you absolutely have to.