drawing relative to different planes

john_blow

I'm wonder if it's possible to draw part views relative to their own faces, rather than the three principle sketch planes.  I'm trying to draw parts and dimension them but since the parts are at an angle to every plane my drawings can't be used for this purpose.
Thanks!

mthiesmeyer

Hi John,

It is currently not possible to place a view that is relative to an arbitrary plane, this is a somewhat related issue, but you may want to create an improvement request on the right. --->

That being said, I do have some workarounds for you for the time being.

If you cannot change the orientation of your part and continue modeling:

 -Snap a Version of your workspace
 -Create a branch off of that version, this will be your `Orientation` branch
 -Place a Mate connector on the face that you want to be relative to
 -Place a Mate connector on the origin of your Part Studio (you can use the part you are transforming as the owning part)
 -Use Transform -> Transform by mate connectors
 -Select all the parts that you want to transform
 -The `From` mate connector will be the one on your part
 -The `To` mate connector will be the one on the origin
 -You should now be able to make a drawing that accurately captures your part.
 -That drawing can either be made in the `Orientation` workspace, or you can snap a version of that branch and reference it from your main branch.
 -Then, when you make a geometry change in your main branch you simply have to merge that branch into your `Orientation` branch and update your drawings.

Alternatively, if you can model in a different orientation, you could take your existing parts, use the steps above to re-align them, and continue modeling your parts in the new orientation all in your main workspace.

Best,

Mike

NeilCooke

Or you could just use an auxiliary view?

john_blow

unless I'm mistaken the auxiliary view is perpendicular, so if I can't draw relative to the face of the part, the auxiliary views won't get me there.

john_blow

Mike I've worked through your workaround and it does the job, thanks! I have added my vote to the existing improvement request.  The only part I haven't figured is the last two steps - snapping a version of my orientation branch and referencing  it from my main branch so that the new drawing updates as I make changes.  Do you mean snap or export? I think I'm missing something there.
Thanks
John

mthiesmeyer

Hi John,

Sorry about that, when I said `snapping` I just meant creating a version. And I glossed over the end steps a little too much, so i'll outline them in more detail here.

If we are in the `Orientation` workspace and we have our part oriented properly:
   -Use the versions flyout to create a version
   -Go back to your main branch and create a new drawing with no views
   -Select `Insert View` -> `Insert part or assembly`
   -Use the version graph button to insert from V1 of the `Orientation` branch (if you are unfamiliar with the operation the docs are here)
   -Create your other views through projection or insertion

After you have the above setup and you have made changes to your part that you want reflected in your drawing.
You would need to:
   -Merge your main workspace into your `Orientation` branch
   -Save a new version of the `Orientation` branch
   -Go to the drawing tab on your main branch
   -Right click the drawing tab, select 'Update linked document'
   -Select `Update all` from the dialog that pops up.

Unfortunately, due to the slightly convoluted nature of this workaround, you will have to do this everytime you want to see your changes reflected in your drawing.

However, there is another approach you could take which would simplify the update process immensely, and prevent you from needing an `Orientation` branch or versions. This would involve deriving the parts you want to draw into another part studio, using mate connectors to position them as above, and then creating drawings of that part studio. This would allow you to get rid of the `Orientation` branch and makes updating as simple as clicking the orange 'Update' icon. You can find the docs for the derived operation here.

Hope that helps!

Best,

Mike

john_blow

Hi Mike, 
thanks for the explanation! I ended up using the derived / mate connectors approach which as you say is much simpler!  Very good to know, so thanks again
John

Elissa_Ledoux

Faster fix: place your part into an assembly by itself.  Mate one face of the part to the origin.  Then make a drawing of the assembly.

Jake_Rosenfeld

@Elissa_Ledoux

This is much easier nowadays now that we have named views in drawings:
https://www.onshape.com/cad-blog/tech-tip-using-named-views-in-onshape