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sweep obviously incorrect.... how can I do this?

malet_jlmalet_jl Member Posts: 15
edited July 2020 in Community Support
I want to CNC machine some text into wood, and replace the removed wood by another wood type, this means that I need the profile to correspond to the tool I will use
the tool is a V shaped drill in order to allow insertion of the negative 
the project is here : https://cad.onshape.com/documents/a858c2a90e852afea76ee9f5/w/eec0f20f6c4b1765f0a6b3ac/e/303fedf5e43da5322c634dee
i asked support from the team as the sweep tool isn't mathematically correct (a sweep shall create a volume where each section is perpendicular to the sweep path and correspond to the sweep profile)
they continue to say me that everything is fine, while it's obviously not the case... 
I have several issues : 
  1. if I try to sweep using two continuous segments, the sweep fails, while if I do 2 sweeps and then boolean merge them, the result is correct (sweep1 + sweep2 is working but sweep6 that do the same create an error)
  2. if the turn is to sharp, the sweep won't success (even if mathematically this isn't incorrect.... and physically this isn't something that can't be produced....) (sweep8)
  3. if the sweep line present an angle, the sweep will fail as in 1) and the workaround of sweeping segment per segment and boolean it don't work since there miss a initial rotation (the profile end tangeant to the previous path and need to be rotated to be tangeant to the starting path... which isn't done and then the result isn't what is expected by a sweep... and doing the rotation by hand isn't an option since it's error prone.... (sweep5)
so what can I do? is there some feature script somewhere that do a mathematically correct sweep?
thanks and regards

Best Answer

Answers

  • tim_hess427tim_hess427 Member Posts: 648 ✭✭✭✭
    Hi @malet_jl - I think there may be a misunderstanding of the purpose of the Onshape sweep tool. It looks like you need is a tool that sweeps a 3D volume along a path. The Onshape sweep tool only sweeps a 2D profile - which creates the issues that you found. Unfortunately, Onshape does not currently have a 3D volume sweep tool (I'm not sure if there's a featurescript or not).

    Do you really need an accurate model of the these shapes? I lot of the CNC software tools I've seen have engraving modes that only require a cutting depth and cutting path, so you wouldn't even need to model all of the sweeps.

    I wish I had a better answer for you, but I hope this helps some. 
  • malet_jlmalet_jl Member Posts: 15
    Hi @malet_jl - I think there may be a misunderstanding of the purpose of the Onshape sweep tool. It looks like you need is a tool that sweeps a 3D volume along a path. The Onshape sweep tool only sweeps a 2D profile - which creates the issues that you found. Unfortunately, Onshape does not currently have a 3D volume sweep tool (I'm not sure if there's a featurescript or not).

    Do you really need an accurate model of the these shapes? I lot of the CNC software tools I've seen have engraving modes that only require a cutting depth and cutting path, so you wouldn't even need to model all of the sweeps.

    I wish I had a better answer for you, but I hope this helps some. 
    hi @tim@tim_hess427
    no I didn't misunderstand the sweep tool, I used a 3D object, because you can move it, while a 2D graph can't be moved.... so I move the 3D shape to the start of the spline, then create a drawing at this place (but looks like the normal of the graph isn't the tangent of the spline, which will create a wrong shape since it has an angle) then I project the 3D object to the 2D graph plane to get the profile and I sweep the profile.... and yes a feature script that do that would be awesome because of the lack of "transform" a 2D drawing....

    I'm not sure about the capabilities of CNC software to perform what I need... in particular the positive has to have a depth that is shorter because of the glue, and "usable" part of the positive is in fact upper because of the insertion angle... it's first time I try this... if the tool do follow the path "on the axis of the tool", the negative will  fit the positive only with a big depth offset... engraving isn't the same as inserting since engraving don't care about the tool result... doing straight engraving isn't difficult.
    maybe I should check if the cnc gcode generator can handle this, but I think that it's a too specifict use to be handled by a tool
    thanks for the reply,
  • malet_jlmalet_jl Member Posts: 15
    in this case, since your cutter is conical, can't you just extrude it all straight and apply a draft that matches the angle of the cone?

    I did the following here. does this do what you want?
    1. Extrude the letter curves
    2. move face by the radius of the cutter (it would be ideal if this offset was already captured in the sketch curves instead)
    3. draft all of the faces by 6.66, the angle of the conical cutter.
    4. use a variable fillet on all vertical sharp edges. Set the main radius to 3mm (cutter radius) and the bottom point of each one to "0.92244/2 mm" (radius of bottom of cutter)
    5. fillet the bottom edge of the extrude by 0.5mm (cutter tip radius)
    I'd recommend setting up variables for your cutter so that it all can be updated in one place later if you decide to use a different one. Am I close to the result you want here? It's going to be a lot of manual work if so.
    hi @Evan_Reese
    this wasn't the way I would have ever thought of doing it, first before sweeping, I tried drafting but it created too many errors.... moving the face... what a CLEVER idea! 
    lot of work, but do-able! much less than my move, project, sweep.... 
  • Evan_ReeseEvan_Reese Member Posts: 2,060 PRO
    @malet_jl
    I hope it works out for you! it's definitely not an ideal workflow, but at least it gets you what you're looking for. I definitely recommend trying to offset the curves themselves instead of the Move Face if you're able. For example, you could probably do the offsets, and warping the text Adobe Illustrator, then export as a .dxf if you're into that kind of thing. I also definitely want to reiterate the value of setting up custom variables to define your cutter too so you can change it without re-doing all the manual work you're facing.
    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
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