[tom.jelly]

Ok, I made some progress today with Kenny's method, I am able to get thru the first and second tool change and they worked fine. The third tool is the shortest of the 5 used for this part, and it has an offset of -.97". The machine hit the z up limit when doing cycle start for that tool change, which is weird because if that was going to happen I would have expected it with tools longer not shorter, than the reference tool. As an experiment I started over and put in an offset of -.56 for that tool and it worked, running thru the program above the height it's supposed to be at by .41" as expected. The rest of the tool changes, with longer tools, worked fine. So I've narrowed down the problem but I'm still not sure whats causing it, any ideas?

[Kenny Duval]

My tool table is set up just as Kenny described. Tool #0 has zero offset, and all other tools have offsets relative to tool #0.

The drawback (as opposed to measuring all tools relative to machine zero) is that if your reference tool changes, you have to remeasure your entire tool collection.

I picked that method as my original machine had a touch probe and touch plate and using the master tool method just made things easy and consistent. Really it's all about which method you want to learn and put into your noodle. On the new machine I don't have a probe or touch plate but still use the master tool method. I just have a DTI in a tool holder as the master tool and then measure my tools off a height gauge I made similar to the Edge Technologies units.

[tom.jelly]

Duplicating a reference tool would be no problem with a height gauge and tool fixture, so that's not really an issue for me. I just need to figure out why the short tool triggered the +z move...BTW what screenset is that in the video?

[Kenny Duval]

Duplicating a reference tool would be no problem with a height gauge and tool fixture, so that's not really an issue for me. I just need to figure out why the short tool triggered the +z move...BTW what screenset is that in the video?

Mach Standard Mill - > Calypso Ventures, Inc.

[machinehop5]

N1 G20 G64
N2 (2 5FL FACE MILL)
N3 G91 G28 Z0
N4 G90
N5 T12 M06
N6 S3094 M03
N7 G90 G54 G00 X-2.1 Y-.8
N8 G43 Z.1 H12 M08
N9 G01 Z-.05 F5.
N10 G17 X0 F75.
N11 X5.75 F100.
N12 X6.85
N13 G02 Y-1.95 I0 J-.575
N14 G01 X5.75
N15 X0
N16 X-2.1 F75.
N17 G00 Z.1
N18 Z1. M09
N19 G91 G28 Z0
N20 G90
N21 (3/4 EM CRB 4FL 1-1/2 LOC)
N22 T04 M06
N23 S3560 M03
N24 G90 G54 G00 X-.185 Y-2.935
N25 G43 Z.05 H04 M08
N26 G01 Z-.2 F6.764
N27 Y-.2467 F27.0558

Is it possible the G43 is causing problems?...I noticed there were no G49 before the next TC, which is common industry format.
https://www.machsupport.com/forum/in...?topic=33793.0

...also read some where about the H code on a line by its self.

[tom.jelly]

I thought the H code just had to be on a line OTHER than the T#, but I may be wrong...I'm also not using the stock SW CAM mach3 post because mach3 wouldn't even get through the code at all with a ton of errors, of course that may be a contributing factor. I can see I'll soon be getting more heavily into G code, but I see G43 is modal; does that mean if there is no G49 and another G43 is called as in the code sample I provided that there would be an issue like ADDING the offsets together? (maybe causing problems if the previous one is negative and the to be called tool one is positive or vice versa) In any case, should the G49 be placed just before each next G43 in the program? Because I can do that until I learn how to edit the post if that might be the issue....

[Kenny Duval]

I don't think there is ever a need for call G44 when using the master tool method. A G43 to call an offset and then a G49 to cancel it should be all that is needed.

[tom.jelly]

Presumably a negative value for G43 would cover G44, no?

[machinehop5]

This a quote from the Mach4 manual...."In writing G Code programs there are some rules to be aware of as well as some general formatting guidelines that should be followed or at least considered.
The first part of any program should be a safe start up block. This line of code is used to make sure that some modes are disabled and others are set to their most common setting. An example safe start block would look like this:
G00 G90 G17 G54 G40 G49 G80
4
This block of code tells the machine that we want to be in rapid mode and using absolute position in the XY plane of fixture offset 1. At the same time we want to cancel any tool diameter and length offsets and make sure any active canned cycles are cancelled.
G00 – Rapid mode
G90 – Absolute position mode
G17 – XY plane select
G54 – Fixture offset 1
G40 – Cutter compensation (tool diameter) cancel
G49 – Length offset cancel
G80 – Canned cycle cancel
It is recommended that this safe start block be used at the start of the program and also before or immediately following every tool change. It is common to restart a program from a tool change, having the safe start line there can greatly reduce the chance of a machine not acting as expected, the results of which can be aggravating at best and a crash at worst. The safe start block shown here is just an example. Every machine and every programmer are a little different and each will have their own start up block."

[tom.jelly]

I'll see if I can figure out if the other posts treat the tool changes differently, but for now I was actually able to get the part to complete, thanks to everyone for their help.

[machinehop5]

I don't think there is ever a need for call G44 when using the master tool method.

interesting I didn't know G44 was Tool Length Offset -- Enable and G43 is + Enable ...there is where the problem thats going on I'll bet.. Using your Post Process editor...you should be able Edit / Replace/ search and replace text in the whole file.

[Kenny Duval]

I think there may be some legacy going on related to this. Perhaps some of the earlier controls could not have a negative value entered into them as an offset. That would lead to a situation where the numbers entered were always positive and the control only new it was negative if a G44 was called. I haven't been involved in it long enough to know that for sure but being a 1's and 0's guy I could see that having been a limitation at some point in the past.

[machinehop5]

back to the passed

[CitizenOfDreams]

start block be used at the start of the program and also before or immediately following every tool change. It is common to restart a program from a tool change, having the safe start line there can greatly reduce the chance of a machine not acting as expected

A proper tool change subroutine MUST leave all the modes intact because it could be called anywhere in the program. It would be crazy if you had to insert G20 after every tool change in case the tool change macro switched the machine to millimeters (although I have heard of that happening in some Chinese control).

[mactec54]

OK so I spent some more time today trying to straighten this out. I homed z to machine coordinates zero. I then switched to part coordinates, touched my ref tool that has an actual gauge line height to tip of 3.6825 and got, lets say 2" and entered the 2" into the tool table, then lifted z up enough to swap to the next tool (#12, 2" face mill with a 3.2" height from the gauge line) and lowered z to touch that one off and got, say 2.4825", which I put in the tool table for tool #12. I repeated for the next tool. I then touched tool 12 to the part surface, set work coordinate z dro to zero, and loaded the G-code in my first post and hit cycle start. the machine z rose to z-.1 for the tool change and requested cycle start to proceed, then ran right in to the upper z limit AGAIN. I then tried other tool heights for tool 12, positive and negative numbers from ,5 to 4 with the same result. The ONLY way the machine will work is to go to offsets tab and turn off work offsets so the light is off. What other issue could be causing this? Note that my machine has fairly limited Z travel because its really a knee mill, so I have to have soft limits of +0.2 soft max and -5.0 soft min, G28 home location coordinate of -0.1, which I will change to -1.0 next to see what happens. The limit switch is at about z+0.3, which I'm sure it would hit if I didn't have soft limits engaged.
Does the actual tool height for each tool even matter after any one tool in the table is touched off? mach should really only care about the DIFFERENCE in height between the touched off tool, regardless of tool number, and the next tool in the spindle, correct? Presumably the tool height is what is entered is only because its more convenient, or am I missing something (something that is kicking my ass, apparently)

Your problem is / was in your program N3 G91 G28 Z0 this will take the Z axis up to machine Zero ( Home in your case ) setup some soft limits this will help not to go all the way up to the limit, and remove this line of code N3 G91 G28 Z0

If ( T12M6 ) is working correct it will move up to the tool change position

You don't have much Z axis travel with these machines so you have to come up with a max retract I used .2 from the limit, so it would never go up and hit the limit

[mactec54]

This a quote from the Mach4 manual...."In writing G Code programs there are some rules to be aware of as well as some general formatting guidelines that should be followed or at least considered.
The first part of any program should be a safe start up block. This line of code is used to make sure that some modes are disabled and others are set to their most common setting. An example safe start block would look like this:
G00 G90 G17 G54 G40 G49 G80
4
This block of code tells the machine that we want to be in rapid mode and using absolute position in the XY plane of fixture offset 1. At the same time we want to cancel any tool diameter and length offsets and make sure any active canned cycles are cancelled.
G00 – Rapid mode
G90 – Absolute position mode
G17 – XY plane select
G54 – Fixture offset 1
G40 – Cutter compensation (tool diameter) cancel
G49 – Length offset cancel
G80 – Canned cycle cancel
It is recommended that this safe start block be used at the start of the program and also before or immediately following every tool change. It is common to restart a program from a tool change, having the safe start line there can greatly reduce the chance of a machine not acting as expected, the results of which can be aggravating at best and a crash at worst. The safe start block shown here is just an example. Every machine and every programmer are a little different and each will have their own start up block."

You never want to use a G49 in the Program Header

[machinehop5]

You never want to use a G49 in the Program Header

Then, someone needs to rewrite the Mach2 , 3, and 4 manual's.

[CitizenOfDreams]

Then, someone needs to rewrite the Mach2 , 3, and 4 manual's.

This time I agree with Mactec. Imagine you have a single-tool program with no tool changes. You currently have some active offset that you don't care about (since you are not going to change any tools). You zero your tool, run the program, the program resets the offset and plunges two inches into the table.

[machinehop5]

This time I agree with Mactec. Imagine you have a single-tool program with no tool changes. You currently have some active offset that you don't care about (since you are not going to change any tools). You zero your tool, run the program, the program resets the offset and plunges two inches into the table.

We are talking about G49 right?

[CitizenOfDreams]

We are talking about G49 right?

Yes, G49, "Cancel tool length compensation". I can see a situation where a G49 in the program header could lead to a crash. I do not see a situation where a G49 in the header would be useful.