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How do I cut constant depth slots into a compound radius surface?

I have an exact model of a somewhat complicated guitar (actually my favorite mandolin) fretboard into which I want to mill slots for the fret wires. I have a sketch showing where I want the slots (the rungs of the ladder) and a line 1/10" inch from the edge. I added one line on the left and I'd like a slot projected (extruded? slotted?) onto the curved surface below do a constant depth of 1/10" .

I added an overview and a closeup picture.

I'm a raw novice at OnShape and I have to say I am very pleased (surprised actually) to have gotten this far. In particular the extrude and revolve let me get the compound curve done properly so I can project the lines straight down onto the curve and the geometry stays correct. Many on the Internet have gotten this wrong and while doing the math is hard OnShape is not. 

I need to take each of all the lines and project them straight down on whatever curve they hit. No curves, cones, nor splines. Maybe I need to move the "ladder" sketch to another plane without spoiling what I have done already? Is there a slot command someplace? Is this a wrap? Is the depth a constraint?

This is the point where I am stuck. A little help will save a novice like me a lot of time.
 
Here is the overview. Notice that I added one line to a sketch using construction lines as a guide. Twenty two more to go.



Closeup showing curve and line line:

Best Answer

Answers

  • bruce_williamsbruce_williams Member, Developers Posts: 790 PRO
    edited September 30
    Hi @tim_collins980 and welcome to Onshape and the Forum!

    You have a good start.  Make sure to check out the 'Learning Center' and help for specific commands.

    It is good to share a public document for the best help.  

    You may do these by making a drive curve on the surface and then Sweeping the groove.  One way to make the drive curve is to Extrude a surface to the face.  Then sketch the Sweep profile on the end of the drive curve (create Plane with Curve point and then sketch profile coincident to drive curve).


    www.accuratepattern.com
  • bruce_williamsbruce_williams Member, Developers Posts: 790 PRO

    www.accuratepattern.com
  • SethFSethF Member Posts: 32 PRO
    edited September 30
    It's best if you include a link to a document that you've made public so people on the forum can make a copy and more easily help out.

    This is probably not the cleanest workflow, but I think it could get you where you need to go: https://cad.onshape.com/documents/7fa9d6888b59ba29c91a2eaa/v/6652f89e0ee650acf9961865/e/5e4b48843abe73195e0917d0

    1) Make a sketch to reference for mate connectors - one on each side of the slot you want to make
    2) Use split the face of the fingerboard at each of those places
    3) Use move face on all the slots to cut away at a constant depth
    4) Close up the ends of all the slots. Probably with a different method than what I did (like just an extrude from the side, or a sweep along the edge).
  • tim_collins980tim_collins980 Member Posts: 5
    edited October 1
    The link (I hope) to the model -- which is public -- is https://cad.onshape.com/documents/3d3d4045af59d97c1db2331d/w/1e62cbc8427c8e3c04b5569d/e/3c430b3e056d3c5124b7333b 

    As an experiment I added a slot-shaped rectangle to the sketch and extruded a hole all the way through where the slot should be. The part is drawn below the "Top" face. Basically I aligned the outside edge of a cone to give the radii and did an intersection. The slot as drawn has parallel sides only.

    @bruce_williams I struggle with terminology, not all your phrases come up in google.  So... I make a plane parallel to the "right" plane such that the new plane passes through the center of the slot. Something extruded would show the surface of the slot perfectly.  If sweep works like I think then I could scoop out the slot to the right depth.   However, I don't see how I can Extrude a surface to a face and do something other than make a hole (see my playing below.) Ideally I would want to project a line onto the face of the curved slab but I think perhaps wrongly that Extrude wants a closed shape. 

    @SethF If I do lots of "splits" along the "right" plane side I would get curved slots with ridges on the bottom where the slots "pushed out" 1/10" of material, and lots of gaps to fill (using two intersections, say.)  The bottom ridges could be cleaned up with a third intersection. Not as elegant as the sweep, but I don't really care what the shape of the bottom of the slot looks like.

    I will experiment with both. I hope that I put the work below rather than above the "top" plane doesn't cause an issue.


  • SethFSethF Member Posts: 32 PRO
    Accepted Answer
    I'm not sure I understand the issue you're describing at the ends of the frets, but I did come up with a decent method for making curves to follow with sweeps. I made a plane proportionally offset from where the nut would be, split the surface, and then patterned the plane and split along the neck.

    Here's my example: https://cad.onshape.com/documents/7fa9d6888b59ba29c91a2eaa/v/5ad6d9b2e0b04772f0d45c41/e/5e4b48843abe73195e0917d0



  • tim_collins980tim_collins980 Member Posts: 5
    @SetF Thank you for making such a large advance in this project. I was using a spreadsheet and hand editing constraints one at a time for the fret spacing. Your document has the actual formula. I extruded and intersected an over-size cone to get the radius. The pattern command is much more powerful and I will learn that next I think (after I do a completely new document.) It is possible that I can finish this project with your help. Thank you.

    The start and end profiles for the nut and bridge ends are different for a compound radius fretboard. The top centerline stays the same height above the bottom of the slab. As the radius increases, there is more sidewall remaining on the bridge end than on the nut end. I will constrain the height to 1/4" and the width (which is a taper) only and let the radius do what it wants to the sides.

    The slots accommodate a tang. To make a tang the bottom of the "T" shape profile metal wire is filed off. You leave an overhang consisting of the exposed top of the fret only. This leaves the sides of the wood intact. It looks better and may be required if there is a decorative element added (binding.)  If I can't do a tang for the first iteration I will drop it for now. That said, I think it should be possible to stop the slots at the two lines drawn 1/10" from the edges.

    One idea I had for making the depth of the slots 1/10" is to extrude and remove a rectangle, per slot, that is 0.023" wide (depends on the fret wire chosen) all the way through. Then add back a copy of the original fretboard that is constrained to be 1/10" shorter and constrained to match the bottom of the original.  This should give slots that have constant depth along the entire length. I've already used those features which may be their only advantage.

    Alternately is to learn the sweep, assuming I can constrain it to stop 1/10" from the edges.

    This is an important model for a wide range of people making musical instruments including not just guitars and mandolins, but banjos and even the violin family (leave off the frets I suppose!)
  • SethFSethF Member Posts: 32 PRO
    I was pretty sure you wanted to close up those ends. I think even if you couldn't find a way to pattern the slots easily, you should be able to easily fill in that area with a sweep.

    I did end up getting what I think is a solution. I couldn't get a sweep to pattern well, so I instead I used more planes for face splits.

    1) Inside the pattern, make two offset planes from the original fret line plane (each offset half of whatever you want the cut width to be)
    2) Use these two new planes in place of the centerline plane for splitting the fingerboard face.
    3) Use a move face to cut down whatever depth you want.

    Here's my example:
    https://cad.onshape.com/documents/7fa9d6888b59ba29c91a2eaa/v/6b2b846e29467473f0abe50b/e/5e4b48843abe73195e0917d0

    But your intersect idea with the cone gave me an idea.
    https://cad.onshape.com/documents/7fa9d6888b59ba29c91a2eaa/v/dd040e1605c448248ae85b36/e/5e4b48843abe73195e0917d0

    This uses thicken and a boolean, which might be a bit cleaner? The boolean tool might be easier to modify.
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