Author Topic: 3D chamfering  (Read 10782 times)

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1612
    • View Profile
3D chamfering
« on: November 20, 2014, 12:43:16 pm »
I recently had the problem of chamfering the edge of a 3D part.  In this case the edge was created as the intersection of two cylinders where the chamfer is needed for welding them together.  I had created a 3D model of the part as an STL file, so within CB I used the Edit/Surface/Edge Detect function to extract a 3D polyline of the intersecting line.  After deleting everything but this line I aligned it and could use the Engrave MOP to follow it in 3 dimensions.  Setting the target depth and using a 90-degree chamfer bit allowed control of the chamfer size.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 5211
  • Made in England
    • View Profile
Re: 3D chamfering
« Reply #1 on: November 20, 2014, 12:55:34 pm »
Very interesting, I've never used the edge detect function but now I know I need to at some point.
How did you align the parts accurately on the machine before cutting ?
Filmed in Supermarionation

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 7295
    • View Profile
    • Cambam V1.0 French Doc
Re: 3D chamfering
« Reply #2 on: November 20, 2014, 13:58:56 pm »
Hello,

Same method for me ; in this case the the purple line is used with an engraving MOP, that give the blue toolpath.
The purple line is done from a line given by the edge detect, the this line is offsetted by using the scale tool (unfortunately the offset tool don't work in 3D, he flatten the line ... and the engraving MOP has no "Roughing clearance" property)

++
David

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1612
    • View Profile
Re: 3D chamfering
« Reply #3 on: November 20, 2014, 18:36:29 pm »
In the case I cited the alignment of the tube was non critical, so eye-balling it in the vise to align the cut with the polyline orientation was enough.  I aligned the polyline so that its highest points were at Z0 using Edit/Transform/Align.

The scaling that David mentions was needed to avoid cutting with the tip of the chamfer bit.  In my case I just made the circle that defines the diameter of the tube a bit smaller than the actual piece.

The polyline has 142 segments resulting in 142 G1 moves from the MOP.  The number of segments is a function of the mesh size in the STL file.

A roughing clearance for the Engrave MOP would be a nice enhancement.
« Last Edit: November 20, 2014, 18:39:39 pm by kvom »

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 5211
  • Made in England
    • View Profile
Re: 3D chamfering
« Reply #4 on: November 20, 2014, 19:03:01 pm »
In the case I cited the alignment of the tube was non critical, so eye-balling it in the vise to align the cut with the polyline orientation was enough.

I was afraid you would say that, I think accurate alignment of non metallic 3D obects on the cnc machine may require use of a 3D probe.
Filmed in Supermarionation

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 7295
    • View Profile
    • Cambam V1.0 French Doc
Re: 3D chamfering
« Reply #5 on: November 20, 2014, 19:04:14 pm »
Hello,

Quote
A roughing clearance for the Engrave MOP would be a nice enhancement.

Yes sure ... or a profile MOP that follow 3D curves  ;D

++
David

Offline Jeff_Birt

  • CNC Jedi
  • *****
  • Posts: 821
    • View Profile
Re: 3D chamfering
« Reply #6 on: November 20, 2014, 20:32:09 pm »
Quote
I was afraid you would say that, I think accurate alignment of non metallic 3D obects on the cnc machine may require use of a 3D probe.

Huh? Machinist have been using all sorts of methods to align/position stock/objects to machine that have nothing to do with what the object is made from. Ever heard of a 'wiggler' or 'edge finder', etc. You can even put a accurate shaft in the spindle, and incrementally jog up to the side of a piece of stock using a piece of paper/shim stock to test for when the shaft contacts the paper (i.e. using paper as feeler gauge.)

Offline Garyhlucas

  • CNC Jedi
  • *****
  • Posts: 1456
    • View Profile
Re: 3D chamfering
« Reply #7 on: December 01, 2014, 22:30:25 pm »
I don't like paper as a feeler gauge, the tool is close enough to do real damage in an OOPS!.  I pick up edges of parts all the time using a round precision pin between an end mill and a part surface, both on top and on the sides.  I especially like picking up the top of a part that way.  I jog in at high speed stopping about 3/8" above the surface, roll my 3/8" pin back and forth until it just touches, set the z at .375 and I'm done.
Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 5211
  • Made in England
    • View Profile
Re: 3D chamfering
« Reply #8 on: December 01, 2014, 22:48:34 pm »
Quote
I was afraid you would say that, I think accurate alignment of non metallic 3D obects on the cnc machine may require use of a 3D probe.

Huh? Machinist have been using all sorts of methods to align/position stock/objects to machine that have nothing to do with what the object is made from. Ever heard of a 'wiggler' or 'edge finder', etc. You can even put a accurate shaft in the spindle, and incrementally jog up to the side of a piece of stock using a piece of paper/shim stock to test for when the shaft contacts the paper (i.e. using paper as feeler gauge.)

Yes I know that but I meant finding the top surface too. And yes I have a Z plate but for all round easy use a 3D probe would be required, it also has other uses too such as creating a point cloud.
« Last Edit: December 01, 2014, 22:51:19 pm by EddyCurrent »
Filmed in Supermarionation

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1612
    • View Profile
Re: 3D chamfering
« Reply #9 on: December 01, 2014, 22:56:36 pm »
I use a 1" gauge block for zeroing Z.  Same principle as Gary.

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8892
    • View Profile
Re: 3D chamfering
« Reply #10 on: December 01, 2014, 23:15:13 pm »
<G>  I use a much more basic approach. 

I move to a place not in the finished part.  Then I run the tool down to within about a thou' (seen by an LED light placed behind the tool and aimed to show the gap), and work it down by tenths until hand-rotation JUST produces a visible mark (just a mark, not a 'chip').  It's always less than a tenth, pretty much regardless of the stock material.

If the work is brutally hard or I cannot access an unused portion, then I use a gauge block.  Skimming a bit across a hard surface isn't good for the cutter.  Marks aren't good for the customer.

For crude work (like that router I'm working on, which has a basic resolution of 0.005"), I just use the light, and go for a 'blackout' at the tool tips.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"