Cutting dimensions for tubes, parallel to the tube.

S_Laurent

Hi all,

I've encountered a problem with dimensions in drawings : consider a tube cut like this :

The only dimensions I manage to use in the drawing are those :

But our builders need them to be like this, parallel to the tube (made this view in Vectorworks):

Has anyone had that problem too ? Any idea hoy to do it ?

Oliver_Couch

Try using the frame tool. It does this automatically

S_Laurent

Hi Oliver, thank you for your answer.

I am using the frame tool, and I know you can get a cutting list like so :

But you can only reference the tubes in the cutting list, you can't put the dimension directly on them. Our builders work faster when they can directly read the length on the drawing, as they do their own cutting lists.

Oliver_Couch

There's no aligned dimension in drawings (although you can do an aligned measurement in the part studio). There's an improvement request here:

https://forum.onshape.com/discussion/25844/align-dimension-parallel-perpendicular-to-edge-in-drawing

Depending on the level of precision you need, you can get pretty close doing it like this:

Alternatively, if you draw one part per view, you can just re-align your view:

Oliver_Couch

Sorry, third option I just realised to hack around it using a sketch (but a very tedious way to create a dimension):

glen_dewsbury

Here is one way to accomplish this. A separate sketch in the part studio can give some lines for dimensioning. When you get to the drawing show/hide sketches.

https://cad.onshape.com/documents/ac0ecfe4f301c56899904542/w/f485e7914d309ca0473669c7/e/7ed9d30f075ee1fb0c01c09a

Oliver_Couch

rhys_skinner

Here's how I work around this purely in the drawing (no part studio sketch)

1. Within the drawing Draw "2point centerline" line on the edge parallel to the dimension you want, it will snap to the edge
2. Stretch that line beyond the cut end
3. Draw another "2point centerline", first clicking from the vertex at the long end of the cut, secondly hover over the previous line and you find it snaps at 90degrees
4. You can now measure to this second line
5. I also add angle measurement between the two "2point centerline" lines for clarity. Be wary if you change the part this angle will change, you will have to redo it

Another nice point about this is you can dimension the cut angle from this 90degree line, as a typical saw would be set.

MDesign

Seems an "aligned" dimension feature request should be proposed if it hasn't been already . Pick two points then pick a line to be parallel with them click dim location.

S_Laurent

https://forum.onshape.com/discussion/comment/110568#Comment_110568

That's what we end up doing most of the time, but it's quite time consuming !

https://forum.onshape.com/discussion/comment/110597#Comment_110597

I hadn't noticed the perpendicular snapping, this seems to be the fastest method, thank you for the tip !

Thank you all for your answers, I've also upvoted the alignment request. It sure would save a lot of time for us !

Oliver_Couch

@S_Laurent PS. If you have a feature request and you're a paid user it's best to submit it to the support team via a ticket (upvoting the thread doesn't hurt though)

They prioritise tickets from paid users over requests in the forum. And the support team is also the ux team so they triage and manage the improvement requests

You can submit tickets by email, via the 'contact support' button in onshape or at https://onshape.zendesk.com