How to change tool cutting point in CAM?

[WillL84]

Hey all, I'm using Fusion 360 CAM for our new Tormach lathe. Tormach for whatever reason on their parting tool uses the cutting edge on the +Z side. Fusion 360 CAM uses the -Z cutting edge. This obviously causes problems. I don't see any way in 360 to pick the +Z cutting edge instead of the -Z, and the way that Tormach has PathPilot setup it automatically sets the tool to use the +Z edge. See attached pic. The black dot shows on the -Z side and sets the tool path accordingly. Any ideas on how to change this? Thanks

[Steinwerks · Accepted solution]

Well you could cheat it and set it up as a Left handed holder (Holder tab when you edit the tool). Can you provide some documentation for the orientation? Just want to make sure we don't get you an answer that could scrap your parts or damage anything.

[WillL84]

It's set up in a turret (#4) and oriented as shown in my attached image, but 180º flipped on the Z axis (cuts from positive X rather than negative X as shown in the image). I had to do some fiddling with orientation and spindle direction in F360 to get CAM to cut from the +X side with the tools in the correct orientation. When I initially setup the tools in F360 so they look like they're set in the turret F360 was showing the tools in the proper direction but still trying to make tool paths in the wrong direction and causing all sorts of crashes in the CAM simulation.

[Steinwerks]

I'm having a difficult time envisioning what's going wrong here. In your first post there was no mention of X at all. 

A few pieces of insight though: how it appears in the tool setup is irrelevant, only that it is presented to the workpiece correctly. In turning, the centerline of the spindle is X0, there is no X- unless the tool passes the centerline (think facing off a part past the radius of the insert to avoid the nub on the end).

Could you export as a .F3D a test file with the issues you're seeing and attach it here?

[WillL84]

Well I fixed the orientation part for all the tools to the correct X axis position. With the lathe all the turret tools cut on the +X side and all tools that to int o the quick change post cut on the -X side. In the attached picture the tool shows like it would be mounted in the QCTP and cut on the -X but CAM actually has it cutting on the +X axis which is correct. I'm sorry if this is getting confusing.

The only problem I currently have is how to make this tool cut with the +Z edge instead of the -Z edge.

[Steinwerks]

I presume you are replying via email, which does not allow attachments. You'll have to reply via the forum to attach images (which I recommend inserting instead of attaching frankly, that way they are integrated in your post).

[WillL84]

Sorry, I am replying in the forum rather than by email and I was referring to the picture I attached in my first post, sorry for the confusion!

[WillL84]

Ok so I did as you suggested (changing the tool holder to LH instead of RH) and it did exactly what I wanted. Thanks!

[Steinwerks]

Good to hear! 

[jazzy283]

So I also have been battling this with my Tormach lathe. I have cheated to fix it as suggested but I am curious what is "right" and why PathPilot/Tormach doesn't agree with Fusion or vice versa. Any ideas out there?

[WillL84]

I'm not sure which one is right, I'm assuming it's an issue with how Tormach has the cutting point setup in PathPilot. I went to their training class back in January and one thing they made sure I knew was that the parting tool cutting edge was on the backside, rather than the front side (RH rather than LH). Gotta be something with how PathPilot is programmed.

[jazzy283]

Huh that is interesting. I asked them about it and they requested what version of PP I was using...but no response for a few days. Still a mystery. I guess the only way to love forward is to hack it for now. Still would love to know all of the reasons why for educational purposes.

[WillL84]

I was out there the second week of January and took their lathe class and that's what the instructor told me. He said for the parting tool if you're standing looking at the machine it uses the right hand cutting edge. That's also the cutting edge defined by PP. F360 however wants to use the LH edge. I'd like to know the reason for the difference as well. But once you get the tool setup properly in F360 you should never have to worry about it again.

[Steinwerks]

In Fusion this is industry standard: all tools are touched off with the leading edge.

I can understand why Tormach wants to define the parting tool by the back edge as that's the part of the tool defining the back edge of the part that is getting cut off, but that seems like a very insulated and unconsidered view from the perspective of standards already established. Lying to the CAM may be the only way to work around this (and believe me, there's plenty of lying to CAM systems in other packages so don't think this sort of thing is uncommon).

[Anonymous]

I am wondering what version of PathPilot you are running.  I see this in the release notes for V1.9.7 (https://www.tormach.com/uploads/1063/SB0046_PathPilot_Release_Notes_0916A-pdf.html😞

************

Release Date: September 20, 2016

Enhancements: 

• #1238: Changes to touch off for grooving and parting tool touch off. Previously, tool control point was set to the tailstock side when touching off; now, control point is set to the spindle side. All conversational routines have a tool width entry field to account for the change in control point. This was done in response to many customer requests to make touch off easier on grooving/parting tools.

NOTE: Old G-code conversationally created in versions before PathPilot v1.9.7 will not work with a tool touched off in v1.9.7 and later; new G-code conversationally created in v1.9.7 and all future versions will not work with tools touched off in versions v1.9.5 and earlier. If in doubt, touch off your parting/grooving tool again and repost the parting and grooving code.

************

Perhaps if you are running an older version of PathPilot and upgrade it will work as you expect?

Scott

[WillL84]

No I'm running 1.9.8 that was released in January, I've been running that since we got the lathe. I actually went out to the Tormach HQ in January for the lathe class and they said to upgrade to 1.9.8 as soon as I got back (which I did once I finished assembling the lathe), so I don't think that's the issue. I've been using it in CAM as a left-handed tool so it works the way PathPilot is expecting it to. not right, but it works for the time being!

[jazzy283]

Yeah same here. running 1.9.8. Still have to fake it in Fusion as a left handed tool. Maybe I just don't understand the actual convention...anyways it works. Cheers.