Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Using loft tool to extrude off parallel to axis

greg_lucasgreg_lucas Member Posts: 4
I'm trying to design a 3D Printed tool to make it easier for me to mark out steel tube notching for fabrication work I do at home. My idea is a cylinder with one end having a snug fit to the tube OD(i.e. +0.5~1mm) and the other end having a loose fit (+3~4mm) then a series of holes around the wall of the tool so I can insert some pins(2.4mm TIG filler rod) and I'd like the pins to follow the angle of the walls so that at the snug end it pushes down onto the tube for an accurate trace.
In the video it shows how some of the pin holes are failing to generate using the loft tool and some nearby holes get very skinny in the middle rather than the uniform 2.4mm end to end shown on the opposite side of the tool.
I think where my problem exists is the layout of the pin holes, I used the circular pattern sketch tool with the same offset (5mm) from the inner wall on both top and bottom faces to mark out the pin holes, and then same amount of holes on each face (48x) resulting in slightly tighter center measurements on the snug side. I used the same origin point for the prime pin hole (inline with the x axis on the rear of the tool) on both faces.
It's very frustrating not be able to drop all pin holes through in one go like I can using the extrude tool.



I'm getting decent working Onshape in block/circular shapes but I'm fairly new to working out of parallel/perpendicular on any CAD suites so definitely been bumbling my through. Guessing that I'm missing either something very simple or very much less likely might have stumbled across an opportunity for improvement.

https://cad.onshape.com/documents/394f3753ad25301d7e3c693d/w/7618e2c90071d3425d9ade13/e/bc69f69a31c274e21df425e7

Comments

  • matthew_stacymatthew_stacy Member Posts: 295 PRO
    @greg_lucas the loft tool definitely has some idiosyncrasies, like not being able to loft a profile inside a profile to create the hollow hexagonal column in a single feature and the "self-intersecting body" error that you encountered in Loft 4.  I suspect that particular loft twisted, though I can't say why the others didn't.  Not having any vertices in the profile may be part of the problem (no rotational index?).

    I would urge you to explore alternatives to the loft tool.  You don't need to loft/remove a gazillion holes around the perimeter of these parts.  Loft/remove one hole.  Then create a feature pattern.

    Also note that by lofting the hexagonal body before extruding the end plates further simplifies the modeling sequence (extrude face of the loft directly, without explicitly creating additional sketches).


    Good luck!
  • matthew_stacymatthew_stacy Member Posts: 295 PRO
    @greg_lucas, after playing with the loft tool a bit more I confirmed that TWIST is indeed the problem that you encountered on Loft 4.  Generally it is best practice for both loft profiles to have the same number of vertices.  There is an option to "Match Connections" to manually tell Onshape how to clock the profiles with respect to each other (often the software default selection is correct ... but not always).  Your model is an example where Onshape needed a little help from a large-brained biped (that's you).  But don't let it go to your head:  Onshape can do lot's of things that you and I can't.



    You are lofting circular profiles which are unique in that there are zero vertices.  So we need to create them.  Just add a point on the circumference of each sketch circle.  Clock them in the same direction (e.g. 12:00) and select them in the MATCH CONNECTIONS option within the LOFT tool. 

    Alternatively, let's explore the effect of intentionally twisting this lofted solid.  I know that sounds crazy, but treat failure as a learning opportunity.  I added a Part Studio to the document (https://cad.onshape.com/documents/583c378d8643ce2d095dcece/w/d20845726b4d6e9a22b7ee6d/e/fc05b324939ff373a5d8aba0 ) with a variable called "twist". Enter larger angle values until the loft feature fails.  Any angle less that 180 degrees works fine.  As soon as you hit that 180 degree threshold the loft tool will give you that self-intersecting body error.  Imagine twisting a paper tube.  Eventually tube will collapse in on itself and fail.  Onshape is showing you the computational analog of that same effect.



  • greg_lucasgreg_lucas Member Posts: 4
    @matthew_stacy Thank you very much.

    Looks like I had the right idea but the wrong execution. I'll give it another go now and report back with how I get on.

    Thanks again!

    @greg_lucas the loft tool definitely has some idiosyncrasies, like not being able to loft a profile inside a profile to create the hollow hexagonal column in a single feature and the "self-intersecting body" error that you encountered in Loft 4.  I suspect that particular loft twisted, though I can't say why the others didn't.  Not having any vertices in the profile may be part of the problem (no rotational index?).

    I would urge you to explore alternatives to the loft tool.  You don't need to loft/remove a gazillion holes around the perimeter of these parts.  Loft/remove one hole.  Then create a feature pattern.

    Also note that by lofting the hexagonal body before extruding the end plates further simplifies the modeling sequence (extrude face of the loft directly, without explicitly creating additional sketches).
    This part especially is where I was going wrong, I was using the extra sketches to brute force the loft tool to do what I wanted it to, but going through your work flow it looks like I missed a step in the loft instructional for selecting profiles.

    (
    Select profiles (a region, face, edge, or point) and then optional cross-sections (in order of the loft direction) and finally the end (region, face, edge, or point).

    To select a set of tangentially connected curves as a single chain, click the arrow next to the desired selection in the dialog to expand the selection field. (A blue field is an active field.) Select more curves to create a composite selection.)




    Good luck!

  • greg_lucasgreg_lucas Member Posts: 4
    @matthew_stacy Followed your advice and had a much better time, I was able to flesh out the design closer to what I had in my head as well.

    Thanks very much for the help.

    https://cad.onshape.com/documents/bbe7469c47815d8388fedcb8/w/16e2bace75322a36341735d9/e/af2ad35add8df93087e7dad9
  • matthew_stacymatthew_stacy Member Posts: 295 PRO
    @greg_lucas, nice work.  No RED!
Sign In or Register to comment.