Calypso CNC User Forums

Have a problem with getting master tool mode to work. This is not a MSM issue, I'm sure its an operator doesn't know what he's doing issue.

Working on my first program. I issue a T1 M06 to load the probe tool. I load it, and using the msm probing screen to find the corner of the piece
in my vise and set x,y,z to 0. This works great.
Then I issue a T2 M06 to load my face mill. MSM says TL0 is on. I load it, and issue the coordinates where I want to start milling. The Z depth is correct for the probe tool, instead of
the face mill.

Most obvious problem would be what I entered in the tool table. I measured all the tools offline. T1 is the master tool and is set that way in MSM and Master tool mode shows on.
But what TLO should I have entered in the tool table? The probe is set to -4.017. The face mill is set to -3.257.

When I single step the code - the WC offset page indicates first -4.017, then it changes to -3.257 so I would think the height is fine, but the Z height of the spindle is too high, and matches
where I would want to be if the face mill was the same height as the probe tool.

The first couple of test lines of code are below. Where am I screwing up?

G90 G20 G94 G43
T1 M06 (change to probe tool and find 0,0,0)
T2 M06 (change to cutting tool)
S3000 M3 (start spindle)
G90 G43 G54 G00 X0 Y0 Z1
Y-0.5 Z-0.0078 (Move down for the first cut)
G91 G01 F15.0 X5.0

Thanks, Bruce

Hi Bruce,

bprager wrote:Have a problem with getting master tool mode to work. This is not a MSM issue, I'm sure its an operator doesn't know what he's doing issue.

Working on my first program. I issue a T1 M06 to load the probe tool. I load it, and using the msm probing screen to find the corner of the piece
in my vise and set x,y,z to 0. This works great.
Then I issue a T2 M06 to load my face mill. MSM says TL0 is on.
I load it, and issue the coordinates where I want to start milling. The Z depth is correct for the probe tool, instead of
the face mill.

I bet the code only did 1/2 of what is necessary for the tool change and APPLICATION of the TLO value for the new tool.
Once you turn on TLO (G43), it will be on and the screens will show that TLO is active. BUT - that does not mean that you have the correct TLO value active, just that some TLO value is active.
The M6 sequence in Mach does not magically apply the TLO value for the tool mounted by the M6.
You have to also go a G43 to change the TLO value from that for the previous tool to the value for the new tool.

consider this:
G49 (turn off TLO)
T1 M6 (this get tool 1 physically mounted)
G43 H1 (apply the TLO value from row 1 of the tool table - which is usually where folks store the TLO value for T#1)
T2 M6 (physically mount tool #2)
(Note that at this point you have T@ mounted and the TLO for T1 active!)
G43 H2 (now the control has the correct TLO value for T2)

This is why many people try to make the tool change line be:
T# M6 G43 H# - which would work fine, except that mach has a long standing bug (See MSM release notes) that causes this to not work correctly when it is all on one line.
Therefore, The bet thing to do in mach is to make all tool change sequences be:
T# M6
G43 h#
as a two line set.

bprager wrote: G90 G20 G94 G43

If this is intended to be the program"Safety line" that sets things to an initial known state, then you want G49 here instead of G43. G49 turns off TLO, while G43 turns it on.
Most programs start with TLO off (G49)

Even if you do mean to start with TLO ON, it's not good form to use G43 without a H register number.
IMHO, that should be a syntax error - but mach tries to help out and guesses at a H# to use - but a control guessing what values to use is, IMHO, a really, really, bad idea.

Consider: Since this is the start of a program, probably the control has just been turned on, what TLO value is mach using since you did not tell it the H register???

Get in the habit of always providing the H register with the G43 and you will avoid any surprises.

bprager wrote: T1 M06 (change to probe tool and find 0,0,0)
T2 M06 (change to cutting tool)

Here you have created the mismatched TLO value situation described above.

bprager wrote: S3000 M3 (start spindle)
G90 G43 G54 G00 X0 Y0 Z1

This should apply the TLO value - but which TLO value (as the H register was not given)?
(I know what mach picked as the H register, but since I don't want to encourage that programming behavior, I"m not telling... )

Ok, that takes care of the G43 related programming issues that I see.

The other problem may be, as you noted, that you may not have the correct values for TLO in the tool table.
Since you are using MSM's Master tool mode (MTM), the key thing to remember is that the TLO value for tool #n must always be the difference between the Master tool's (MT) physical length (PTL) and the physical length of tool #n.

This is why, in MTM, the TLO value for the MT, will always = 0. Because MT PTL - MT PTL = 0.

Please see chapter 9 of the MSM user manual for pictures of these tool length relationships and how the TLO values are calculated with MT mode.


BTW, since you are probing to set the corner zero etc, you have a probe interfaced to the machine OK.

With the latest release of MSM you can also easily add a touch plate at the tool change position (without needing more interface electronics) - I would recommend thinking about doing that. Then you can forget all about how the values are calculated and getting the right numbers into the tool table etc - just let MSM measure the tool when it is mounted and it will handle all this for you. I'm a strong believer in making the machine do the tedious work for you.

Dave

Thanks so much. This was one of those problems where I knew I had read/seen what I was doing wrong, but just couldn't nail it down.

As soon as I saw the H1, I knew that was what was bothering me.

I like the tool plate idea, but am using a Tormach, so I will have to see how I add in another device. The current probe tool is connected to an external probe socket they provide.

Not sure if any other pins are available or if I have to add in some kind of board to the PC.

But I agree that the touch plate option is the way to go, especially since I will have to do a lot of drilling so that way I can measure the bits as I mount them.

Thanks again. Great help as always!

Bruce

Hi,

bprager wrote: I like the tool plate idea, but am using a Tormach, so I will have to see how I add in another device. The current probe tool is connected to an external probe socket they provide.

Not sure if any other pins are available or if I have to add in some kind of board to the PC.

The all software solution that MSM 2.0.10 offers does require a 2nd pin be available on the breakout board. I am not familiar with the pin outs of the Tormach breakout board, so can't help with that detail.

If there is not a 2nd pin available, you can combine the probe and touch plate lines with some electronics and feed the composite signal into the current probe connector pin. This is what had to be done before I invented the software only solution - see section 6 of the MSM manual for info on the electronics approach.

Dave