How to Change/Edit Parts Without Disabling Mates

loic_billaut

I am new to Onshape and can't figure out how to edit parts of an assembly without creating errors for mates associated with that part. 

Perhaps I am not creating mates in a way that would allow me to edit the parts associated to it? I have tried creating mates in the part studio too but that doesn't seem to solve the problem of the mates not automatically connecting in the assembly. 

For example, in the attached image all connections between the top/bottom boards and vertical bars are revolute mates. If the vertical bars are rotated to the horizontal position the boards will thus come together. In this assembly, if the vertical bars are extruded downwards to be longer and create a larger gap between the boards, the revolute mates between the bottom board and vertical bars will be red and "unsolvable". I then need to go into editing each of those mates to re-mate the mate connectors. 

I would greatly appreciate any help in regards to making edits to parts without creating errors for the mates connected to that part. 

Thanks 

john_mcclary

A mate needs to reference some part of the geometry of your part. If you edit the part so much that the entity you mated to has been removed/replaced.

Example: you mate to the edge of a part. Then you edit that edge to have a fillet. The edge has been replaced by two edges and a curve face. All with new unique internal I.D.s

Adding mates in a part studio is the best way around this.
But do not confuse mate connectors with mates!

"Mate connectors" are points in space that are attached to a part or geometry.
"Mates" need 2 mate connectors as input. The Type of mate determines what movement is allowed.

So when you add mate connectors in a part studio, you will need to actually mate them in the assembly.
When you do this, they will never break unless they have broken in the part studio. Or the part itself got a new internal I.D.

loic_billaut

Thank you !

I don't know what an I.D. is ... could you explain that to me?

I also tried a simpler experiment to figure out how to edit parts without dismantling the mates in the assembly. In this one I extruded the core downwards (similarly to how I extruded the vertical bars downward) but in this case the mate in the assembly adjusted accordingly and didn't dismantle or show any error.



Maybe it worked because I extruded on the same axis as the mate connector? Also the part I was editing (the vertical bar) appears 4 times in the assembly. Maybe the software adjusts the mates one by one which would create "unsolvable" errors momentarily but cannot recognize that there is no longer a problem?

Just taking a shot in the dark...

Thanks

john_mcclary

The ID is a randomly generated number that every entity gets assigned on creation. 

It's how a computer knows what object you are manipulating. 

So if you have a cube, you will have a list of IDs that defines it

Imagine:

Part 1 (ddd3b5bxfkk78)
Edge1 (htedu7736bj63)
Edge2 (dhe88mx3xb2b)
Face1 (hh4bb6xx7mm2)
Ect...

So if you fillet edge1
You are really pointing to the id (htedu7736bj63)
Now if you delete the extrude feature that made part1 and remake it
.
It gets a new random number and so do all of the edges and faces. 

Some features could use the input part duplicate it, delete the original. Then you would have what looks like an identical part. But all of the internal ids would be suddenly different. And all your mates would still be looking for a part with the old id

loic_billaut

Thanks, that helped a lot!

I tried editing the bars again this time trying not to add or replace any features, and it worked perfectly.

Thanks again!