Partial extrude remove using text sketch

lars_rengersen

In my design I want to add text to indicate some info. My laser cutting company will interpret holes/cutouts that are not all the way through as engraving (and this is what I am after).
So on the surface I want such an engraving I added a sketch and used text.
However, while extruding that I only get 'all the way through' results.
My sheet metal is 1 mm tick and even if I set the extrude remove to 0.2 mm only, it goes all the way through.
Any suggestions on what I am doing wrong or what other approach I could take?
Thanks in advance for any input.

Jake_Rosenfeld

@lars_rengersen

Currently our sheet metal only allows cuts all the way through.  You can do this kind of cut if you "Finish" the sheet metal first.

This limitation is on our radar, but it would be helpful if you went to the "Improvement Requests" section of this forum and created an improvement request for this feature.

philip_thomas

@lars_rengersen - If you post a public link, it will be fixed in 5 minutes!

The short answer is that when you extrude an entire sketch, its the outer boundaries of each profile that are used.
You would need to select the regions to extrude to leave the centers.

Post a link and watch the forum race to fix it for you!

Jake_Rosenfeld

@lars_rengersen

Currently our sheet metal only allows cuts all the way through.  You can do this kind of cut if you "Finish" the sheet metal first.

This limitation is on our radar, but it would be helpful if you went to the "Improvement Requests" section of this forum and created an improvement request for this feature.

Jake_Rosenfeld

@lars_rengersen

I have a workaround for you! Here's what you need to do:

1. Make a new assembly
2. Insert the flattened version of your part into the new assembly
3. Click the "Create Part Studio in context" button in your assembly (It's the last button on the toolbar and looks like the Part Studio icon with a '+' over it)
4. Select the assembly origin as the origin and click the check mark.  You'll now be brought to a new Part Studio with a transparent version of your flattened part.
5. Use the 'Transform' feature with the 'Copy in place' option to get a copy of the flattened geometry.
6. Engrave as desired.
7. Hit the 'Insert and go back to assembly' to make it associative.

At this point, your assembly will look a little weird (two overlapping versions of the same geometry, one engraved and one not), but the upside is that solution is fully associative!  If you make changes in the original part studio, go to the in-context part studio, use the context switcher to switch from 'None' to 'Context 1', and hit the '...' menu, then 'Update Context'.

Please let us know if you have any questions!
https://cad.onshape.com/documents/01a4c795bbe8df5e955e3634/w/853fddca0e6cd22868ea3e4d/e/ea5f2795be88e105eb1ee002

https://www.onshape.com/videos/design-in-context
https://cad.onshape.com/help/Content/in-context.htm

lars_rengersen

Jake_Rosenfeld said:

@lars_rengersen

You can do this kind of cut if you "Finish" the sheet metal first.

Thanks! That helped and works fine for me. Good to hear that half way through extrusions are on your radar as a future improvement. I'll search for an improvement request for this one and if yes vote on it or otherwise I'll raise it.


Thanks also for adding the workaround in a second response. Finishing the sheet metal first was easier for me.

oliver_august

Hi, I stumbled over the same topic just now.

@lars_rengersen , did you start an improvement request back then?

I just wanted to ask if this matter might be solved in the meantime?
Or does it still only work using the above mentioned workaround?

glen_dewsbury

Jake_Rosenfeld said:

@lars_rengersen

Currently our sheet metal only allows cuts all the way through.  You can do this kind of cut if you "Finish" the sheet metal first.

This limitation is on our radar, but it would be helpful if you went to the "Improvement Requests" section of this forum and created an improvement request for this feature.

Here is a IR from 2017.
https://forum.onshape.com/discussion/7312/0/#Form_Comment