Basic Part Creation for Assembly

[nomar116]

I am trying to model a multi-hinged rock climbing cam. The design is essentially three overlapping hinged pieces. My problem is I've tried a number of ways to create these pieces so they match-up correctly in an assembly.


I found making theparts individually meant I had no way to match the surfaces when I was creating the next part. Its a three part set so I made two successfully but they seem useless because the third piece has to be "cut" from the assembly...if that makes sense.


I went back and started over, drawing one part with several surfaces atvariousdepths for each of the three parts I would need to cut from this template. This seemed to work, but the frustrating problem I'm encountering is LOTS of errors when trying to make a cut. Usually they say "part and feature must intersect" and some others (sorry its late). It seems the heirarchy of protrusions is making overlapping cuts very difficult...I'm soo confused.


Is there a way to copy a sketch, protrusion, or section from one part and import it into another? Or is there anyway to edit one part using a different part to constrain in the sketcher? Thanks for ANY help!!

 

[appinmi]

You can copy geometry from one part to another. On the top tool bar, select Insert, Shared Data, Copy geometry from other model.

 

[nomar116]

I am just dying here.


I did that and sure enough it worked to import the geometry. BUT Now I can't get rid of the geometry after I've drawn the part to be connected to it. Is there a way to alter the parent/child relationships or something so that I can remove this geometry? Making a cut to remove it didn't work either, it executed the cut but didn't actually CUT anything!

 

[appinmi]

Create the boundaries of the new part first. Then, instead of Copy Geometry from Other Model, select Cutout from Other Model.

 

[Dell_Boy]

You can copy features and sketches from one part to another WITHOUT creating dependencies using Edit/Feature Operations/Copy/FromDifModel


DB

 

[dr_gallup]

You can also create your part cuts in assembly mode. You just pick the part in the assembly window and RMB Activate. Now you are working on the part in the context of the assembly. If you want to reference geometry from the other parts you will have to allow external references.

 

[denisvragolan]

Hi, nomar116.


It is not clear to me what you want to do, but maybe this approach can help you.


Memeber "apimni" told you that you can copy geometry from another model. If you copy surfaces, you can "solidify" them. So, you have to:


copy surfaces


View attachment 2249


create solid geometry


View attachment 2250


select surface(s) and activate "solidify"


View attachment 2251


and set it to remove excessive "material" of your solid...


...and here you are


View attachment 2252


I hope this helps.