2D Chamfer CAM something is wrong

[JonSchaeffer]

2D Chamfer is taking the chamfer width I enter and adding that same amount in z which crashes into floors.

It never used to do this. 

We used to just enter the Chamfer width, (.010)

And enter the tip offset and it did exactly that and still created the .010 chamfer.

It never used to add to the z value.

[seth.madore]

Well that is odd...

Can you share your part, either here or privately (PM)?

What is your Height selection set to?

[JonSchaeffer]

I couldn't share the part.

But I re created the issue. Took a few screen shots, and I am uploading this Fusion file too.

The distance to the floor I am chamfering is .060

I entered .050 for the Chamfer tip offset this should stay .010 off the floor.

And the last 3 photos show the geometry I picked, then the tool path going all the way to the floor of the part. And then a photo showing the simulated tool. 

[seth.madore]

I'm 99.99% certain that the behavior exhibited in the above file is as it's always been. Chamfer width + Offset amount = final z depth of tool. To reduce any gouging that may occur, reduce the amount of offset.

[JonSchaeffer]

Hi Seth, No sir it didn't used to be this way. This was one of the best features about Fusion that I loved. It didn't add the chamfer size to the Z depth, It auto calculated it's radial step over to achieve the chamfer size. And because of the radial step over and the super awesome "Chamfer Clearance" feature, you could bring the body of the tool as close to a wall as you wanted. It gave you that control. (I know this because) This  was an older post that I had on why I couldn't use cutter comp inside 2D Chamfer. Because I found out the option for cutter comp/Wear was disabled even though the option to turn on Wear was there. The G code would not put in G41. It was explained to me Fusion couldn't control a sidewall crash if they allowed the Wear feature to work, which is why I had so much control on my tool paths. My tool did not dig into a floor of a part and I didn't hit side walls. Super powerful. Lars Christensen has a video teaching on this chamfer technique. Other wise having a 2D chamfer operation would make no sense. It would work just like using the Contour tool path for a chamfer like we did in the old days. You would need to pull out the calculator and give it your Z offset and stock to leave would be a "minus value" 

[seth.madore]

Alright then, I will look into this. Thank you for the detailed response. Is it your sense that it was behaving differently as early as before the last patch, or is this something that's been plaguing you for a bit?

[JonSchaeffer]

I am super sorry I didn't report this earlier. I have been super busy with deadlines and kept working through the issue. I wish I could tell you the exact update I found out about it. The  closet I can recall was, I did report an issue with the Drilling command. I modeled my chamfers on holes and I used a spot drill and selected the surface of the chamfer on jobs so I would not need to calculate Z depth. Well after an update that feature wasn't working correctly and when I had those jobs become repeat jobs, I had many parts scrap out my first articles, because it sent my spot drill really deep. 

I will look up that report date. Maybe this would be a good indicator since it has something to do with chamfers.

[JonSchaeffer]

11/8/18 Was the day I reported the spot drill issue. Hope this helps.

[seth.madore]

Sadly, the spot drilling and faces issue was a whole other mess we found ourselves in. I'll do some poking today (if time allows) and see if I can find an older build that exhibits different behavior

[JonSchaeffer]

Thank you Seth! I sure appreciate all you vested time with this! 

[Jon_Bancroft]

@seth.madore

For as long as I've been using Fusion, ~2016, the 2D chamfer operation has always added chamfer size plus tip offset for the final Z depth as you said. A 0.010 chamfer with 0.010 tip offset would put the chamfer tool 0.020 below the selected edge. The screenshots posted above are behaving as they always have for me, 0.05+0.01=0.06.

[JonSchaeffer]

I have been a Fusion 360 user since the beginning. I am an early adopter. 

I could be fooling myself... maybe I am wrong on this, BUT... I am pretty sure I remember doing some chamfers on a part that had a very shallow floor. Which required me to control the depth so I did not run into my floor. 

It does not make sense to choose a tip depth and it automatically adds the chamfer size to that depth. 

The user looses all control at this point. And it also makes creating a 2D chamfer cycle not needed. 

We might as well go back to using contour and do it like we did old school early CAM and tell the software all the calculated depths and step over amounts to create the needed chamfer.

If we have a Tip Depth option to control, it should be exactly that.

Then by the entry of chamfer size tells the system it should move over "radially" The CAM should calculate the same amount as Tip Depth "Minus" the chamfer size. Then we have depth control and perfect chamfer sizes.

[Jon_Bancroft]

I agree that your description is how it "should be done", offsetting the tool radially to get your chamfer width at a fixed tip depth.

However, as I said my Fusion experience has always been chamfer width plus tip offset is total tip depth.

With the past two January updates I have lost many of my Fusion preferences and CAM "defaults" each time, resetting me to a default CAM environment. And this weekend with that latest update freshly installed, which again wiped my defaults, my chamfer code still behaved as I described.

I would much rather it work the way you described, but this has been like this for me since long before last November.

[JonSchaeffer]

Thank you for the agreement in how it should function. 🙂

[JonSchaeffer]

@seth.madore  Any word on a possible fix for this?

[seth.madore]

Sorry for the delay in responding. It took longer then I expected to to gain access to an older version of Fusion. I went as far back as last July and well, the behavior is the same. I'm sorry to have to tell you that. 😞

Here are some screenshots. The step is .100 deep, the chamfer is .01, and the offset is set to .100". You can see that the depth goes to .110", gouging the part. Ahha! A bug! Yes, but that still exists in current release. This becomes visible when we set our tip diameter to 0. It doesn't seem to be able to calculate collision with a zero sized tip. Setting the tip to anything else results in the aforementioned toolpath failing. The closest I can get is to a -.0899" and .010" chamfer.

Bottom line: As far back as last July, the depth of the tool was "chamfer size + offset"

If you have another installation date in mind, let me know and I'll try to run it through that as well.

[CGPM]

This is the way I remember it working for as long as I have been using the software, which was the first trial release to a controlled test group.