Workflow? Master Sketches / inheriting sketch elements from another sketch in the same part studio

andrew_kleinert

I'm having problems using master sketches.  In this case, I'm trying to create master sketches in two different planes, and there are elements of the master sketch in plane 2 that I want to inherit from the sketch in plane 1.   

I've created a simple example below to model a hamburger.  I've created a master sketch on the front plane.  I'm using the master sketch to work out the high level dimensions and proportions of the hamburger.  Individual sketches are then used for the individual 'parts' and any fine details.

It would be helpful to be able to create a second master sketch on the right plane, which I could then inherit the outline of the bun, the pineapple, and the patty from the front plane master sketch.  And I could then use the right plane master sketch to control the outline of the cheese (assuming the cheese slice is rectangular not square).  

I can copy elements between different sketches, but it doesn't retain the symbolic link.

I can derive sketches between parts studios but it doesn't allow me to do it within the same part studio.  I can create a new sketch in a new part studio, 'use' the elements from the derived sketch, but I can't derive the new sketch back in the new part studio to the original part studio: Error message "Operation failed because it would create cyclical references"  (BTW, I think that message should say "circular references" rather than "cyclical references"?)  

In some cases, I can project lines to the intersection of the two planes, but that can't be done in all cases.  And in the cases when it can, it often clutters up the master sketches in a way that would be nice to avoid.

I could use variables (and I do), but that can be difficult to manage when the number of sketch elements gets large.  

The '=' operation doesn't seem to work between lines in orthogonal planes.

Is there a way of easily working with orthogonal master sketches in Onshape?  If not, is it a useful feature request?  (Are others trying to follow this workflow?)

Obviously this is massive overkill for a simple project like this hamburger, but for more complex projects that have many more parts, it feels like it could be useful?



Link to project: https://cad.onshape.com/documents/8e0f118093af4784a6d42b80/w/dee7478121d12b7475dc9032/e/54d6fd0d1b71c6e5d80c2c6a?renderMode=0&uiState=6204997d7e2a0d6e6ff148fa

eric_pesty

You could do a 90deg circular pattern of your first sketch (from the front plane) to get a "copy" of it on the right plane, that way you could reference it and/or do equal dimensions etc on a sketch on the Right plane...
The "=" uses "projected" lengths so the length is going to be zero on a perpendicular (front to right) plane, but you should be able to pickup the bun outlines on a top plane sketch using coincident (can't do pierce if out of plane).

S1mon

I do this sort of orthogonal sketching to lay things out all the time. It’s easy to use constraints to make the second sketch dependent on the first. I’m not sure where you would need to use derive. I do miss 3D sketcher tools from Solidworks which allow you to make things equal or aligned in more flexible ways, but even with just 2D orthographic views you can construct just about anything geometrically.

Maybe I’m missing something but I can’t really see where the challenge is.

andrew_kleinert

S1mon said:

It’s easy to use constraints to make the second sketch dependent on the first.

For two sketches that are on orthogonal planes, how do you use constraints to make the second sketch dependent on the first? 

andrew_kleinert

eric_pesty said:

You could do a 90deg circular pattern of your first sketch (from the front plane) to get a "copy" of it on the right plane, that way you could reference it and/or do equal dimensions etc on a sketch on the Right plane...

Aha, that's awesome, thank-you!

Didn't realise it was possible to do a circular pattern of a sketch.  Works a treat!

andrew_kleinert

@lougallo not sure if it's intended behaviour or not  ...

... but when a sketch has been patterned (as @eric_pesty described above using 'circular pattern') it doesn't follow the 'Hide other sketches' / 'Show all sketches' commands.

eric_pesty

@andrew_kleinert
The visibility behavior is consistent, when a "feature" creates sketches, planes, etc...
You have to toggle them by showing/hiding the "feature" (there will be an "eye" icon to the right when mousing over) that created them. But it would be nice if they followed the general show/hide all commands, improvement request?

andrew_kleinert

eric_pesty said:

@andrew_kleinert
The visibility behavior is consistent, when a "feature" creates sketches, planes, etc...
You have to toggle them by showing/hiding the "feature" (there will be an "eye" icon to the right when mousing over) that created them. But it would be nice if they followed the general show/hide all commands, improvement request?

Agreed 👍