MTM-TLOs

[JimsMSM]

Dave, Trying to load TLOs into the tool-tbl using Master Tool Mode on my Tormach--all Tools are RH. I'm using a Tool-Setter I made which lights up the Probe-LED when touched. My Settings are:
"Settings" page: TLO G-Blk is TP is ON, TCP-TP-Installed is ON, Max Dist: 10.0 for both Touch and TC-Pos
"Tooling" page: G43 (TLO-Active) is ON, Master-T-Mode is ON, Master-Tool # = 1

I jogged the MT to the touch-plate (tool-setter) and hit "Save-Pos'n) which zeros Z. When I MDI: T2 M6, then hit "Measure-Tool" or "Set-TP-TLO" the Spindle returns to the TCP, then I get an error msg: "MaxZDist <= MinProbeDistance, Op Canceled"

My Tool-Setter/TP is below the TCP. I'm trying to follow Para 9.1.4.2 "MTM TLOs using TCPTP.

Appreciate any info you can provide?
Thank You Much

[DaveCVI]

I jogged the MT to the touch-plate (tool-setter) and hit "Save-Pos'n) which zeros Z.

Are you trying to set the TCP position at this step?
The next panel to the right, the "CPos'n to TCP" button will set the TCP position to whatever the current position is of the spindle (in machine coordinates).

The two buttons in the "curr Position" panel are independent of tool chagnes etc - the "Save Pos'n" button simply stores the current position, and then you can jog around and the "Return Pos'n" button takes you back to the saved position - however that saved temp position is totally independent of the TCP. These buttons were inherited from the 1024 screen set - just so they would be present - frankly, I don't think I've used them since they were implemented - and I don't remember what path is taken from current position to stored position - probably a straight line.

When I MDI: T2 M6, then hit "Measure-Tool" or "Set-TP-TLO" the Spindle returns to the TCP, then I get an error msg: "MaxZDist <= MinProbeDistance, Op Canceled"

My Tool-Setter/TP is below the TCP. I'm trying to follow Para 9.1.4.2 "MTM TLOs using TCPTP.

Appreciate any info you can provide?
Thank You Much

The secret to remember is that moving the tool to the TCP TP is really a probe operation internally. I.e. the tool is "probed" to the TCP TP - then the probe input line triggers, the tool stops and the software reads the MC position to get the tool length info it needs. Now here is the secret: since this is a probe operation, it uses the probe parameters as set on the WC Offset, Probing page.

Go look at the "Max Z Distance" DRO in the "Probing Op Parameters" panel on that page... I'm betting that it's set to 0.
Probes to the TCP TP are allowed to go the minimum of Probe Max Z distance and the Max dist from the setting page. Yeah, That's a bit less intuitive in hindsight than I'd like

Dave

[JimsMSM]

Setting the WC-Offset Probing Max Z-Dist and Probe Fast FR did the job; however, ran into another head-scratcher:
I set the TLOs on 10 different RH tools, checked the tool-table report and all looks good. I used the MT to touch off and set Z0 on a test part. Then did a test G-code prgm that calls for three TCs and to touch the part with three different length tools. All three tools did not touch the part, all were approx 6mm above the part which is the TLO of the first tool change (the second tool is approx 6mm shorter than the MT). Then tried touching one of the other test tools (all non-MT) and reset Z0 and that tool and the remaining tools worked great. It's like if I use the MT to do the initial part touch-off and set Z0, the remaining tools don't make it to the part, but if I use any non-MT to touch-off and set Z0 -- they all work.
Here's how I put the TC code in the prgm: T2 M06 G43 H2 Z0.0 (this is what my CAM prgm generates). I also added a M1706 but don't see any difference with that.
Again--appreciate your time.

[DaveCVI]

Hi,

...
Here's how I put the TC code in the prgm: T2 M06 G43 H2 Z0.0 (this is what my CAM prgm generates).
...

Again--appreciate your time.

I'd bet the G-Code tool change line is the problem - I think you've hit a known Mach bug.
Please see the MSM release notes item 4.27 for more information.
The solution is to change the post processor to generate a two line tool change - like this:
T2 M06
G43 H2
Z0.0

The Z move can probably be on the G43 line, but since mach has bugs in this area, I'd make it be on the next line after the G43.

Dave

[JimsMSM]

That Did It--Working Great--Thank You Much
I'm Lovin MSM !!!