Cutter Comp/Wear Compensation

[brysny]

I'm having trouble getting wear compensation to work. From reading about Mach3 it sounds like cutter diameter wear is not used, only the cutter diameter is used. But from the MSM manual it sounds like MSM has routines that extend the mach tool table functionality and use the wear info.

I generally have my CAM program use the nominal tool diameter and correct all toolpaths. But for tweaking dimensions a few thou I want to be able to adjust via G42/G43. From reading about Mach3 functionality it sounds like you can do this and put either a small positive or a small negative number in for the cutter diameter and the one funny thing it does is for a negative number it actually will just reverse the mode and use the absolute value (so a -0.002 dia with G43 is implemented as 0.002 and G42 turned on).

But if I try putting either a negative tool dia, or have a tool dia of zero and put in a wear value with MSM I get an error message saying 'physical tool diameter must be >=0 '. Also it triggers a bug where even if you then try and set the tool diameter to positive the message pops up and the values don't get stored.

Seems like a bug that MSM is forcing the tool diameter to be positive, or is it that Mach3 doesn't handle this and so MSM is just protecting the user?

My setup is:

MSM v2.0.0 , Mach v3.043.062 , winXP 32, shuttle pro plugin

[brysny]

Slight correction. When you start with a new tool, the first time you enter diameter information that results in a negative physical size (ie your cam did the primary comp, but the cutter is slightly worn) things work as expected. But then if you try and edit the tool you get stuck with the MSM error of 'physical tool diameter must be >=0 ' and it will not save any of the edited data no matter what you put in.

[DaveCVI]

Hi,
Oh my, you did ask an interesting question....

The MSM code for the dialog that that edits the tool table is doing
"If Diam + Wear) < 0 Then ...."

I suspect that I just wrote that as a sanity test for dialog input data before saving values into the tool table.

I bet my thinking was along the lines that a tool has a physical diameter, and in the real world that has to be a + value. The tool can wear, but it can't wear down past a 0 diameter (at least not until the shop is on a space shop traveling at warp speed or some other such fun )... so if the sum of diam + wear < 0, the user must have mistyped a digit or something.... Seemed logical at the time.

But that logic assumes the values are really representing a physical object's diameter. If instead, we look at the values as just numbers to be used to offset a path, well, then as you have pointed out, there may be cases where the total diam+wear could be < 0.

Frankly, I could see making either argument.

For context, I looked at my design notes and I don't have any explicit notes about what mach does if it is handed a net cutter diam that is < 0. I don't think I've ever tried that.

I could weaken the MSM test, and let one just feed mach the raw numbers, then mach will do whatever it does (and I'm uncertain I want to know that that is in this case.... see below). If I did that in MSM, I think I'd change the "oh no you don't" to a "well, OK, but here's a warning message in the log file in case you really didn't know what you were doing".

I'm a bit less certain after thinking about this tidbit you supplied....

Jul 24, 2012 10:51:59 GMT -8 brysny said:

From reading about Mach3 functionality it sounds like you can do this and put either a small positive or a small negative number in for the cutter diameter and the one funny thing it does is for a negative number it actually will just reverse the mode and use the absolute value (so a -0.002 dia with G43 is implemented as 0.002 and G42 turned on).

Did you mean to write that as G41 (CC left) and G42 (cc right)?
I'm confused as G41/G42 pair for CC and G43 (positive TLO) and G44 (negative TLO) pair for TLO offsets.
But you wrote G43 (positive TLO) changes to G42 (CC right) and that threw me.... ??

I'll assume you meant G41/G42 since the topic is cutter comp and wear values.

But teh news that mach does this scares me a bit. I can see mach doing it (it's consistent with mach's tendency to "help out too much" and think that it knows better than the g-code programmer what was intended). But it's a state machine violation for the g-code program if mach actually does that.

My concern is that when I program a G41, I expect to get a G41 modal state. I do not expect mach to change G41 to G42 and change the sign of the value entered and sneakily use a value that was not explicitly programmed. That creates a situation where mach is putting the gcode interpreter into state that is NOT the one that was programmed by the programmer. I consider that bad mojo....

Of course, while I personally think that is undesirable behavior for a g-code interpreter, as the author of MSM I **could** choose to ignore that and just call it "that's the way mach works" - (Doc, it hurts when I do this.... then don't do that" ).

So.... if I take out the diam+wear < 0 test, and this leads the user to cause mach to do G42 when G41 (or vise versa) was what the program said it wanted.... am I just leading users by the hand to get bit by this?

I think I'd like more input from others before I do anything rash here re MSM's diam value test -

Dave

[brysny]

Hey Dave,

Yes I spaced there for a sec and meant G41/G42. Also on whether or not mach switches modes in order to always use a positive comp, that is something that I read on the mach forum and not something I was able to verify. I can try some more tests though.

In terms of how the cutter comp is used, it is very standard now for even low end cam packages to do cutter comp at the computer and output paths that account for tool diameter. Most also have the option to still output G41/G42 to allow for 'wear' adjustments. In reality this can be anything from the actual tool diameter being off, to tool runout, to backlash, to fixture stiffness, etc. But when used this way the numbers are small, a few thou usually, and are just as often negative as positive.

In a production shop setup there is usually a programmer and an operator and so the operator or the setup tech would be the one tweak the wear dia and it would be a major issue if they had to go back to the programmer to have the programmed tool diameter tweaked. It is also bad practice since the next time the job is run it might be a new tool and so would then need yet another code change. Considering that most MSM users are probably programmer and operator in one it is less of an issue, but still a hassle since you generally need your cam program on another pc than mach so it can still be running back and forth.

Also in regards to leaving MSM as is, it currently does have a bug. It allows you to put in a negative entry the first time you edit the tool and does not pop up any message at all. Then the second time the message comes up, and it repeatedly comes up even if you make the diameter positive. So you have to reload another tool table to wipe it out.

I think a clean solution would be to turn the message into only a warning (and have it pop up the first time). Then it would be up to the user to decide if that was the intent.

Regardless, I appreciate your dang near immediate response and also the well thought out nature of it.

Bryan

[DaveCVI]

I'll think about this some more from the MSM viewpoint. I'm going to ignore what mach may or may not do with a negative net diameter (Mach is what it is...)

FYI - It'll be late in the week or next week before I can shake some time free for this.

In the mean time, If anyone else has some opinions re this, I'll be listening....

Dave

[mattster1]

Hello,

I am new to the forums but have been in the industry for quite awhile programming cnc machines using CAM software in 3, 4 and 5 axis formats. When we first started (back in the day) the method was to us the radial dimension of the tool at the control and program to the feature size. However with the smart machine controls and reliability of the current CAM packages plus the introduction of better simulations in the CAM packages, the prefered method, at least in a majority of the shops in our area, is to use the CAM package to offset the tool starting the register value at 0 (Zero) and use a negative (for tool wear) and a positive at times (runout etc.) to adjust the tool path at the control.

It really comes down to your preference and programming method or CAM access. But seeing as how you asked for input I figured I would join in. My vote with the cam access and habits I have gotten used to would be to be able to input a negative number.

FYI
While I am experienced in the later model industrial controls I am a bit of a newb on the bench top controls and how to tweak them so I will be doing a fair share of "listening" and hope I can at some point be able to provide some constructive input to help others.
I just accquired a SYIL speedmaster X5 with 4 axis capability and a 24K watercooled spindle.

Matt

[DaveCVI]

Hi Matt,
Welcome and thanks for the additional input.
I've put the ability to set a negative total diam in a beta version of MSM.

It should show up in a public release not too long from now (I've also got some other minor changes that I need to complete testing before a release).

Lurk all you want, and feel free to ask questions - we'll do our best to answer.

Dave

[DaveCVI]

FYI - the tool diameter test changes are in the MSM 2.0.4 release.
Dave