How to delete extruded parts

jamie_o_shea478

So I'm creating a Dice Tower which needs to be able to have a 19x19x19mm dice drop.  So my issue is that I am not sure how to remove the extruded parts that stick out of the main cylinder so that it is flush.  Not sure if using thicken, may have been more successful, and I tried using things other than blind, but it didn't work.  Thanks in advance.

https://cad.onshape.com/documents/df5548c28396ac7cde420cbc/w/dfa0a60ddb57e4e7b3b15b6d/e/15f0ff2ccefe7c8eaeac7a08

larry_hawes

Can't open the doc...

Jake_Rosenfeld

@jamie_o_shea478

Does that document still exist?  Is it a public document?  I cannot seem to access it either.

See instructions here:
https://forum.onshape.com/discussion/9107/forum-post-checklist#latest

jamie_o_shea478

I didn't make the document public, fixed it now.  Thanks in advance.

larry_hawes

Jamie, I don't know why those extrudes weren't being cut by the walls of your tube but I copied your Bumper extrude to the Right plane (in the middle of your tube) and extruded in both directions. It seemed to behave better. I am really curious as to why your first attempt extended like it did, and how one would would fix that. 

https://cad.onshape.com/documents/ce0986315feda4e166ef804f/w/56749476f1fb8f180c136365/e/ca8ed633fb1f162b138d457e

owen_sparks

I can see a couple of options.

(1) Delete face function. Help here

(2) Split the part using its outer cylindrical face and then use delete part to get rid of the unwanted bits. Then boolean the good bits back together.

Hope that helps,

Owen S.

larry_hawes

Owen did you try either of those options? I cannot figure out how to use either function in that document...

Jake_Rosenfeld

@larry_hawes

Here is an example using both of @owen_sparks suggestions:
https://cad.onshape.com/documents/410b3697489d02fe7003cf0b/w/ae79883ed9d2f1f9baf0b17e/e/a2bd25856114210204f9dc8c

larry_hawes

Thank you Jake,

Figured out the delete face feature but it needs to be accomplished very carefully as some faces seem to need fewer selections, others more, and just found it really fiddly.

Also got the delete part to work but it is so difficult for me to understand the proper order and sequence or which part to split from which part - sheesh - just so fiddly for me to try and grasp the paradigm and technique.

Both are probably simple and straight forward as they should be but I simply could not get the functions to work without help. That may say more about my skills versus the function's er.. function but it really can be frustrating at times.

larry_hawes

Please tell me this is just a little crazy making. It seemed I have to choose EXACTLY the proper face - sometimes all the faces - sometimes not all the faces - in order for ALL the faces to be deleted. Is this something everyone is aware of?

Check out the second extrusion and which faces need to be selected in order for all the faces to be deleted. If I select all the faces it gives an error but if I choose just the correct 2 faces all the other faces are deleted. Seriously? I have to be missing something...

http://www.youtube.com/watch?v=YGTyF5i0ZWg

https://cad.onshape.com/documents/f6b47447e385dcb40393833d/w/d80dd6f4bd55a77d7ed28bcf/e/377776d5d8aa22d1ef0193ed

larry_hawes

I see there was a lot of little faces around the corner of the faces I was not selecting but is there any explanation for the behavior of the second face delete routine where ALL the faces were deleted by simply selecting 2 specific faces?

larry_hawes

Tried it again and found a couple other (seeming) inconsistencies. I'm curious as usual is this document behaving as expected?

http://www.youtube.com/watch?v=qhHzxBy9C1s

https://cad.onshape.com/documents/f6b47447e385dcb40393833d/w/28cc3debae131bcf8ae2538c/e/377776d5d8aa22d1ef0193ed  Branch B1

larry_hawes

Jamie,

I hope this thread is helping you get your model right!!!

Jake_Rosenfeld

Hi @larry_hawes

From your first video, it seems like there is some confusion about the different options in delete face:
https://cad.onshape.com/help/Content/deleteface.htm

I've made a document for you which illustrates the difference between the three options:
https://cad.onshape.com/documents/ec957a9f1e9e053170cc12ee/w/bc8b6acd4f4cf9002b749b50/e/c4933cca30c39b4d13423e6d

"Leave open" can be thought of as the first step of delete face.  As you can see here, leave open deletes the face from the body, and leaves the body as an open surface, rather than a solid part.  You'll notice that this is listed in the parts list as a surface rather than a part.

"Cap" and "Heal" can be thought of as post-processing operations on this open surface.  "Cap" will simply apply a cap over the empty space of the void created by deleting faces.  "Heal" will attempt to extend the surrounding surfaces until they meet.

The behavior you're seeing where you only need to click on two of the faces to delete the entire protrusion is a result of "heal" behavior.  The result of extending and trimming the surrounding surfaces is, in this case, to close up the entire void.

You've asked a few time in your first video "This isn't working, is this even a face?".  Yes,  all the selections you are making are faces.  Our input boxes have smart filters on them such that you can only select the entities that are relevant to the operation (a.k.a. it is impossible to select an edge, vertex, or part into that selection box, the only selections you are allowed to make are faces).  When the operation turns red, it is in indication that the operation is failing.  Failing operations will not make any geometry changes.  In this case, the operation is failing because it is not possible to "heal" the void created by deleting the faces.

For a simple example of a "heal" that will fail, you can try to delete the top face of a cube.  Since all the side faces are straight up and down, no combination of extension or trimming of those faces will produce a solid body, so it is not possible to heal the deletion.

Another small note.  You mention "will this only work if I make this exact set of selections in this exact order?".  In general, order does not matter for selections in Onshape.  There are some exceptions in cases where it is intuitive that the order matters, e.g. loft profiles must be selected in the order that you wish material to travel though them.  In this case, though, the content of your selection matters, but not the order of your selection.

In general, delete face is a direct modeling operation that is useful when there are no other options on the table (e.g. when you are working with imported geometry).  If I were to make this design myself, I would use modeling techniques such as extrude up-to-face to create parametric geometry the first time around rather than overbuilding and having to use delete face.  Other options that are more parametric than delete face here would be revolve cuts or split part.

Hope this helps
Jake

P.S. sorry for the essay

larry_hawes

Thank you for the 'essay' and I appreciate you taking the time to explain some apparent inconsistencies. I have a feeling that some models require some experimentation in order to find just what surfaces need deleting in order to achieve the desired result and I think this can be fairly confusing for a newer using looking for an absolute answer to a process that may not always be straight forward.

Of course your example will be easy and straight forward as they usually are but I have a feeling there will be a few cases where one will have to experiment a bit to get the desired results and find out just when something is healed or not when deleting surfaces.

BTW my first response changed the model as well to include a different strategy for the extrudes so they wouldn't need additional surface deletion steps.

Again thank you for taking your valuable time to respond, I really appreciate it.

Jake_Rosenfeld

@larry_hawes

Just took a look at your first solution.  Very nice!  @jamie_o_shea478 you should definitely check out that first answer (and maybe change "New" to "Add" if you want the whole thing to connect up).

I agree that "Delete face" is a little trial-and-error on more complicated geometry than my contrived example, especially since it's a little hard to tell which faces are already selected and which aren't.  I'll log an improvement for this internally.

larry_hawes

Jake_Rosenfeld said:

@larry_hawes

Just took a look at your first solution.  Very nice!  @jamie_o_shea478 you should definitely check out that first answer (and maybe change "New" to "Add" if you want the whole thing to connect up).

I agree that "Delete face" is a little trial-and-error on more complicated geometry than my contrived example, especially since it's a little hard to tell which faces are already selected and which aren't.  I'll log an improvement for this internally.

Again, Thanks so much for all your help, it does not go unappreciated...

owen_sparks

Jake_Rosenfeld said:

I agree that "Delete face" is a little trial-and-error on more complicated geometry than my contrived example, especially since it's a little hard to tell which faces are already selected and which aren't.  I'll log an improvement for this internally.

I had an IR in for this but it got demoted   

https://forum.onshape.com/discussion/6167/delete-face-highlight-faces-not-edges

Cheers, Owen S.

lougallo

@owen_sparks not really demoted.. just not something that needs to be voted on.  More of a bug or oversight.

owen_sparks

Thanks @lougallo

larry_hawes

I know this thread has run its course but if the OP Jamie returns here's another way to perhaps accomplish your same design without the extrusion changes needed.

https://cad.onshape.com/documents/fa524d8150381e7936389632/w/7d8ab3b4aa822eaaa87e1190/e/d746d044216bd56fe195a5b0