2D contour - actual chamfer tool diameter

[Anonymous]

Hi,

I have get something strange when I use chamfer mill with 2D contour toolpath. I am confused which tool diameter is taken for computation.

2D contour toolpath -  I have selected  tool .375" dia  chamfer mill 45 deg with .01" tip diameter.  When I run it as a contour only without selecting chamfer option (at passes tab) looks like Fusion takes .01" tip diameter as a tool diameter and use it for toolpath calculation. Effect is that tool gets too deep into material and this is not intended.

When CHAMFER option is selected, the software takes actual tool diameter .375" and use it for toolpath calculation.

Is it bug?

Marek

[kate.raskauskas]

Hi @Anonymous,

I tried this with a simple chamfered box and couldn't replicate the problem; can you please post your file so I can take a look?

[Anonymous]

Kate,

Here is attached file.  The last 2 toolpaths.  The first one without selecting chamfer option will crash the part.

Thanks

Marek

[Steinwerks]

2D Contour is calculated via the Tip Diameter of the tool. Selecting the Chamfer option uses the defined taper to calculate the correct geometry.

You can use an expression to set your tip offset to engage the maximum flute length without bottoming out on the shank diameter too. Trying to remember this one specifically so I'll post again when I get it.

Also your geometry selection isn't great. When using 2D Contour with the Chamfer option it's much easier to pick the bottom of the chamfer and use the tip offset to set the bottom of the toolpath.

[Anonymous]

I am trying to finish cylindrical diameter .454  and chamfer depth .075 from the flat face at the same time. Tool will be extended and to avoid vibration I wanted to ramp down. 

[Steinwerks]

The simplest way to do that is probably to use 2D Contour without Chamfer enabled and set Radial Stock to Leave at half the diameter of the tool minus the radius of the tip diameter.

In this case that value would be .1825".

It would appear that using Ramp forces the tool into a Wall Taper Angle situation though and creates a closing helix toolpath. Which is pretty weird.

@fonsecr is this how Ramp is supposed to work with a chamfer mill? Neat, but maybe not always ideal.

[fonsecr]

Yes and no 🙂

I actually have a high priority task pending for this. So the user can choose how to approach with the stepdowns or the ramp. Hope to get to it soon.

[Steinwerks]

Good to hear! I like the taper ramp functionality and can definitely see a use for it, just don't want to be forced into using it if undesired

[Anonymous]

Neal,

I like the idea to use radial stock for this purpose .  Do you know how to use it with formula so I do not have to recalculate it each time?

As fat as a ramp I have noticed that the ramp is "conical" with the chamfer tool, but it does not work in my case.

Thanks

Marek 

[Anonymous]

Neal, just to let you know about expression,I found online, there is a list of variables

https://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/CAM...

[Steinwerks]

I'm well aware of the variables, just haven't had time to dig into it. @tim_paul did a webinar in which he used an expression for using the top edge of the cutter taper but I couldn't find it quickly. Maybe we'll get lucky and he'll pop in and share it here.

[tim_paul]

I hope this helps....

(tool_diameter-tool_tipDiameter)/2-chamferWidth-.005in

[Steinwerks]

Thanks @tim_paul!

I see this is for 90° tools only though, just as a note. Granted that's what's being used here so this could be a solution.

[tim_paul]

This is what I recently started using to place the chamfer right about in the middle of the cutting edge.

((tool_diameter-tool_tipDiameter)/2-(chamferWidth/2))/2

[Anonymous]

Thanks for hint, I can use it in a future.

Unfortunately in this case I wanted to helical ramp down and finish cylindrical diameter at the same time. As it is mentioned earlier, helical ramp in contour behave strange when chamfer tool is selected. 

Marek

[tim_paul]

I see what you're trying to do. Seems reasonable that we could select the outer diameter to compensate from. I also tried a tapered end mill and that didn't work. I HATE to say it, but to get moving forward and to get a good tool path I would use a flat end mill for now and some simple math. @cj.abraham should take a look at this. Maybe I'm missing something or maybe we can get a ticket for this. If I had my way I would like to comp to tool diameter and then be able to bore down to the tapered surface after selecting the wall and the tapered surface. 

Lastly I changed the comp type to in computer and I think I go the result you are looking for if you don't care about comp. 

I hope that helps.

Try this is you want to take a look at what I did

http://a360.co/2sCAchk

[Anonymous]

This is what I did. I have just selected regular flat end mill and used 2D contour with helical ramp down. I had to recalculate depth and double check it to make sure there is no mistake. When I did simulation it looked like tool cuts into material but this is because of the flat endmill. Actual tool will be chamfer mill.  We will run these parts on machine probably this week.

You are right about selecting the "larger" chamfer diameter. I wanted to compensate to it. The tolerance is +/-.002", I am using wear compensation.

The bad thing is that I cannot simulate actual chamfer mill to see if there is no mistake. 

Summarizing, it is doable but takes more time and gives extra opportunity for mistake. I think the helical ramp with chamfer tool should be changed or at least give user option which way he wants to use it.

Thanks

Marek

[Anonymous]

N19T19(3/8" DIA SC CHAMFER MILL 90 DEG INCLUDED ANGLE)
M6

G90 G0 G17 G40 G49 G80 G69
S1324 M3
G54
G0 B50.715
G0 X0.002 Y2.93
G43 H19 Z11.9403

M8
G0 Z3.4403
G1 Z3.0403 F10.
G41 X0.0407 D19
G3 X-0.0408 Z3.0358 I-0.0408
X0.0407 Z3.0313 I0.0408
X-0.0408 Z3.0269 I-0.0408
X0.0407 Z3.0224 I0.0408
X-0.0408 Z3.0179 I-0.0408
X0.0407 Z3.0134 I0.0408
X-0.0408 Z3.009 I-0.0408
X0.0407 Z3.0045 I0.0408
X-0.0408 Z3. I-0.0408
X0.0407 Z2.9956 I0.0408
X-0.0408 Z2.9911 I-0.0408
X0.0407 Z2.9866 I0.0408
X-0.0408 Z2.9821 I-0.0408
X0.0407 Z2.9777 I0.0408
X-0.0408 Z2.9732 I-0.0408
X0.0407 Z2.9687 I0.0408
X-0.0408 Z2.9643 I-0.0408
X0.0407 Z2.9598 I0.0408
X-0.0408 Z2.9553 I-0.0408
X0.0407 Z2.9509 I0.0408
X-0.0408 Z2.9464 I-0.0408
X0.0407 Z2.9419 I0.0408
X-0.0408 Z2.9374 I-0.0408
X0.0407 Z2.933 I0.0408
X-0.0408 Z2.9285 I-0.0408
X0.0407 Z2.924 I0.0408
X-0.0408 Z2.9196 I-0.0408
X0.0407 Z2.9151 I0.0407
X-0.0408 Z2.9106 I-0.0407
X0.0407 Z2.9062 I0.0407
X-0.0408 Z2.9017 I-0.0407
X0.0407 Z2.8972 I0.0407
X-0.0408 Z2.8927 I-0.0407
X0.0407 Z2.8883 I0.0407
X-0.0408 Z2.8838 I-0.0407
X0.0407 Z2.8793 I0.0407
X-0.0408 Z2.8749 I-0.0407
X0.0407 Z2.8704 I0.0407
X-0.0408 Z2.8659 I-0.0407
X0.0407 Z2.8614 I0.0407
X-0.0408 Z2.857 I-0.0407
X0.0407 Z2.8525 I0.0407
X-0.0408 Z2.848 I-0.0407
X0.0407 Z2.8436 I0.0407
X-0.0408 Z2.8391 I-0.0407
X0.0407 Z2.8346 I0.0407
X-0.0408 Z2.8302 I-0.0407
X0.0407 Z2.8257 I0.0407
X-0.0408 Z2.8212 I-0.0407
X-0.0269 Y2.8994 Z2.82 I0.0407
X0.0269 Y2.9606 I0.0269 J0.0306
X-0.0269 Y2.8994 I-0.0269 J-0.0306
G1 G40 X-0.0013 Y2.9285
G0 Z11.9403

M9
G28 G91 Z0.

[Anonymous]

Rene',

Any idea on when this correction is going to be implemented or how to track it?

Thanks

Marek

[fonsecr]

I'll schedule the approach mode feature for the October release. It is long overdue.