MSM Turn help

[civtek]

Hi
I am trying to running MSM Turn but have some problems. What I am trying to do is to set up some tooles with a Master tool as a ref. Then I want to turn a pice and change the tools just to put the tool # in the toolpage when asked for, but I do not manage to set up the tool or call up a tool. Doing a t# in the MDI bar do not result in anything (still remainds 0). I have read the manual and looked at the video but have not managed to get any results here.
I would like a step by step information or iven more, a video shoving how to set up some tools and how to select them when asked for a toolchange.
I also have a mill running the MSM and there everything runs OK.
Thanks
Civtek

[DaveCVI]

Hi,
In any MSM system you have to use the MDI line to change a tool. MSM will not let you type a tool number into the current tool # DRO to do a tool change. This is due to bug in mach; using the MDI line get mach to do things right and avoids the bug associated with the current tool DRO approach (that the mach 1024 screen set allows).

Re actually changing tools on a lathe, I suspect that you are getting stuck on the differences in gcode between mIll mode and lathe mode.

Different gocode commands are used for mill and lathe mode to change tools.
This can be a bit confusing to new lathe users as teh gcode words are the same letters, but the syntax and semantics are very different. Here is short intro to help get past the learning hump:

Mill mode:
In Mill mode you use T# M6 to do a tool change. THe T word selects the # of the next tool to change to. THe M6 says "change to whatever tool is given by the last T word. THe M6 does the physical tool change.
HOWEVER, no TLO value is applied by mach as a result of the M6 action. TLOs become active when you run the G43 H# gcodes. The H word says use the offset from entry # in the tool table. The G43 says apply TLO values starting now.
NOte that this means that there can be any amount of time between when a tool is changed and the TLO values aer applied. Mill mode is fundamentally a 2 step process to change a tool and start using the TLO valeu for the new tool.

Now, mach makes this real y bad as it accepts the M6 word when in lathe mode. That should be an error but mach ignores the error from using a mill mode gfcode in lathe mode.

So what is the correct gcode in lathe mode?
For lathes, the tool change and TLO activation is a single, one step, indivisible operation.
All lathe tool changes and application of offsets are done with the T word only.
In lathe mode it is Txxyy where xx is the tool # to mount and yy is the row # of the tool table to get the tool offset values from.

Thus T1010 will mount tool #10 and apply the offsets from row 10 of the tool table. most mach lathe uses will have xx=yy as they only use one offset for one tool (but that is convention, not a requirement of the gcode).
Note also that you can type odd thing like T102 - is that Tool 1, offset 2 or is that tool 10 offset 2? Avoid that any always get in the habit of using exactly 4 digits for all tool changes... you will not get bit as much and your head will hurt less.

To change a tool in MSM for a lathe, say you want tool #1, use the mdi and type T0101

Dave

[civtek]

Hi
Yes I was messing up turn and mill gcodes. I now can lood a tool but I am not gettig the screens I espekt. I will try to explain.

In the TOOLING PAGE I put T1010 in the MDI bar and hit enter. Next tool 10 shows. In Tool Change box "Tool Change" blinks but NO green arrow appear. TC Status say: Mont Lathe tool.

Then I go to the RUN PAGE. TC (upper right) is blinking. I press cycle start (green arrow) and TC stop blinking.

Back to TOOLING PAGE. And now tool 10 is showing as Current tool and TC Status say: Tool Change Complete
This is surly not the way it should bee working? (The green arrow should have appered when first in the ToolingPage?)

I have another question. I do not have limit switches on my lath and can therfor not do a Homing opperation. In Mach3 one can sett home manualy, can that bee done in MSM to?

Civtek

[DaveCVI]

Hi,

Hi
Yes I was messing up turn and mill gcodes.

I understand - the difference can be confusing when first starting to use a lathe.
Here is a really confusing example of what happens if you use mill gcode in mach's lathe mode.
1) Suppose you typed T03 M6 in the mdi line.
That looks like a valid mill mode tool change, but we in lathe mode so what does mach do?
First mach sees the M6 and ignores it. If the M6 were flagged as a syntax error (invalid Lathe gcode) the user would be stopped here and the problem would be obvious.

2) Now mach will see the T word, and read the # after the T
2) Mach will see that only 2 digits are supplied.
3) mach will use the 2 digits (03) as the tool number.
4) now mach needs an offset #, bu there is not one... so mach will use 00 for the offset index.
5) but "00" is the magic number to say "do not apply any offset".
So instead of an error you will get a valid tool change to lathe tool #3 with no offsets applied...

I now can lood a tool but I am not gettig the screens I espekt. I will try to explain.

In the TOOLING PAGE I put T1010 in the MDI bar and hit enter. Next tool 10 shows. In Tool Change box "Tool Change" blinks but NO green arrow appear. TC Status say: Mont Lathe tool.

Then I go to the RUN PAGE. TC (upper right) is blinking. I press cycle start (green arrow) and TC stop blinking.

Back to TOOLING PAGE. And now tool 10 is showing as Current tool and TC Status say: Tool Change Complete
This is surly not the way it should bee working? (The green arrow should have appered when first in the ToolingPage?)

You are correct, the Tooling page Cycle start button should turn green. The symptom you have described probably results from a known Mach bug. Sometimes Mach does not correctly initialize the brains that MSM uses.

To fix the problem, please see item 4.1 in the MSM release notes. It describes the same problem you have seen and tells you how to fix it.

I have another question. I do not have limit switches on my lath and can therfor not do a Homing opperation. In Mach3 one can sett home manualy, can that bee done in MSM to?

Civtek

It is dangerous to do anything in machine coordinates when you do not have home switches. Without home switches, the machine can not tell where it is in physical space.

The MSM tool change position is stored as machine coordinates. If you ask MSM to go to the tool change position and the machine is not referenced, the movement could crash the machine. This is why MSM refuses to do the goto TCP movement if the machine is not referenced.

Without home switches it is best to not use the MSM tool change features (Go TC Pos'n and TC Auto TCP buttons).

The best solution is to eventually add home switches.
Until then here is what you can do (at your own risk):

If you do not have home switches AND they home switch signals are not defined (enabled) in the mach port&Pins dialog, then whenever mach is asked to home/reference an axis, mach marks the axis as homed and sets machine coordinate 0 to the current position of the axis.

If you do this, when you click ref-all home, each axis will be set to MC0 and the axis labels will turn green. As far as mach is concerned the axes are now referenced. MSM relies on mach to check the axis states - so when MSM asks mach, mach will say that the axes are all referenced and MSM will not know any better.

If you do this, you will have a different physical location for X,Z Machine 0 each time you reference the axes. This can crash the machine if you then tell MSM to go to the TCP, and the TCP location is past the end of the physical travel. you can do this, but you must be aware of what the consequences could be of doing this.

Dave

[civtek]

Hi Dave
Quote:"To fix the problem, please see item 4.1 in the MSM release notes. It describes the same problem you have seen and tells you how to fix it" Yes it did it! Thanks.
A new question. Is it possible to start the cutting operation to the right of the object? As for now the tool start cutting from Z= 0 in the - (minus) direktion. I would like the tool start all cuts at say Z= +2mm to take up the backlash in the leadscrew?

Civtek

[DaveCVI]

Hi,

Hi Dave
Quote:"To fix the problem, please see item 4.1 in the MSM release notes. It describes the same problem you have seen and tells you how to fix it" Yes it did it! Thanks.

Good. Unfortunately, there are many Mach bugs that I've reported to ARtsoft, but they have never fixed them.
The best I can do is document them and hope that someday Mach3 actually gets some attention and they start fixing reported bugs.

A new question. Is it possible to start the cutting operation to the right of the object? As for now the tool start cutting from Z= 0 in the - (minus) direktion. I would like the tool start all cuts at say Z= +2mm to take up the backlash in the leadscrew?

Civtek

The CNC control software (mach3) just makes whatever movements it gets in gcode commands. Therefore the general answer to your question is "yes". But there is no magic way for the control to do this magically for you.
If you are hand writing the gcode you can do this when you make the gcode.
If you arae using a cam program to generate the gcode, then you have to investigate what features the CAM program has.

Dave

[civtek]

Hi Dave

Every thing works fine now. Thanks! But I still have a question. How do you zero the MC axsis? I do not have limit switches as I think I do not need them. Do not use or need the function: GTCP. In my case, do I have to zero the axsis in MC at all?

Civtek

[DaveCVI]

Hi Dave

Every thing works fine now. Thanks! But I still have a question. How do you zero the MC axsis?

Mach will not let you set a MC to zero via a button or script. As far as I know the only way to zero a machine coordinate axis is to reference/home the axis.

Hi Dave
I do not have limit switches as I think I do not need them. Do not use or need the function: GTCP. In my case, do I have to zero the axsis in MC at all?

Civtek

AS long as you don't try to use a function that requires the use of a previously stored machine coordinate, MSM will not care. So if you don't use those you are fine.
If you do try to use one of those, MSM will tell you and try to keep you out of trouble.

Dave