HSM tool path problem on chamfers

[vedadave]

Autodesk Inventor HSM pro 2015
Windows 7 x64
Operation: 2D Circular, Using a ballnose endmill tool to cut chamfers on multiple holes feature tops.

Problem: If 'Hole Bottom' is selected as the bottom height then the tool will not move low enough to cut the full chamfer.

              If 'Hole Bottom - offset' is selected then only one tool path is generated - on the first hole.
              If 'Model Bottom' or other height is selected then no tool paths are generated.

Questions:

1. What is the preferred way to cut such a chamfer if I don't have a correctly sized chamfer tool?

2. Is there a work-around?

[Laurens-3DTechDraw]

Using 3D Contour?

[hansun_zhu]

Hi,

For the failed cases you got, it could be related with the tool size or offset value based on the hole diameter, so could you please try -

1. Use a smaller tool or reduce the offset if possible?

2. Or try to do the chamfer on each hole individually to see whether it can work fine?

3. Or to use 2D Contour with checking "multiple depth" (specify the related taper angle) and the desired offset in bottom height

If you can let us know the tool diameter and the each hole's diameter, it could be better for us to know what the problem is.

Thanks
Hansun

[Laurens-3DTechDraw]

hansun wrote:

Hi, For the failed cases you got, it could be related with the tool size or offset value based on the hole diameter, so could you please try - 1. Use a smaller tool or reduce the offset if possible? 2. Or try to do the chamfer on each hole individually to see whether it can work fine? 3. Or to use 2D Contour with checking "multiple depth" (specify the related taper angle) and the desired offset in bottom height If you can let us know the tool diameter and the each hole's diameter, it could be better for us to know what the problem is. Thanks Hansun

I'm baffled with this response. Since when do 2D operations compensate for the endmill's radius. He is using a bullnose/ballnose he said. And running Inventor HSM Pro. Go 3D!! Easier to program with better results.

[jeff.walters]

If you only have 2D then 2D Contour with multiple depths can work. If you have 3D then you will most likely get better results with 3D contour or maybe even a 3D spiral. The advantage of the 3D toolpaths is that the tool will stay in contact with the part more.

[vedadave]

I tried 3D Contour and it works ok. I had to calculate the bottom depth based on my 3/8" tool and the depth of the chamfer though. Otherwise the the tool path goes all the way to the hole bottom.
2D Circular with a 45 degree chamfer tool works faster but I only have a metric tool and no collet for it.

[lenny_1962]

vedadave wrote:
2D Circular with a 45 degree chamfer tool works faster but I only have a metric tool and no collet for it.

then make an adapter for it, do that all the time, lathe, drill hole, then drill for set screw, then use that in a collet.

[Laurens-3DTechDraw]

vedadave wrote:
I tried 3D Contour and it works ok. I had to calculate the bottom depth based on my 3/8" tool and the depth of the chamfer though. Otherwise the the tool path goes all the way to the hole bottom. 2D Circular with a 45 degree chamfer tool works faster but I only have a metric tool and no collet for it.

You can just select the bottom of the chamfer as your bottom value and give a little negative offset value. It's even quicker than the 2D version especially when you don't give in a boundary but just use the check surface, select the chamfer and turn on touch surface.

[17asleep]

vedadave wrote:
I tried 3D Contour and it works ok. I had to calculate the bottom depth based on my 3/8" tool and the depth of the chamfer though. Otherwise the the tool path goes all the way to the hole bottom. 2D Circular with a 45 degree chamfer tool works faster but I only have a metric tool and no collet for it.

You do realize that non-metric collets can be used on metric shanked tools?