Having problems with tool offsets, machine will only work with them turned off

[tom.jelly]

I'm having a problem trying to get my machine running multiple tools with tool offsets. This is a Boss 5 Bridgeport converted to Mach 3, the machine works fine for parts cut with a single tool zeroed on the stock top. Now I need to incorporate tool changes, here is the procedure I used to set up the tool offset table: I home the machine to machine zero, then I assembled tool 1 with a 1/2" dowel pin as reference tool and measured from the gauge line to tip at 3.6825 using a height gauge on a surface plate with a taper fixture (the 3.6825 is the net length after deducting the height of the fixture) I measured the rest of the tools the same way and then entered the lengths in the tool length column of the tool table and hit enter and apply for each entry.
The first tool I need is tool 12, a face mill that measures 3.2" from gauge line to tip. I zero that face mill to the stock top with a sheet of paper and enter zero on the main program page for mach, z axis, work (not machine) coordinates. (For the purposes of this exercise I am not concerned with the thickness of the paper). I load the g code, regenerate toolpath, press cycle start and the z axis rises to the z axis tool change position of machine coordinate z = zero. Mach says press cycle start after tool change. I already have tool 12 in there, so I hit cycle start but then immediately the z axis raises to the upper limit switch, triggering the estop. Note that the correct tool and associated offset is in the tool information spot on the program run page.
In troubleshooting this if I go to the offsets page and click tool offsets off (the green light off) before hitting cycle start after each tool change, the G code runs fine and there is no problem. I've looked at many videos and instructions,( most of which aren't very specific or gloss over what must be some critical detail) and can't figure out what I'm doing wrong, I'm sure the answer is right in front of me but its not sinking in. Any tips would be appreciated. I have only ever run this particular machine, which I converted and have minimal CAM experience but a lot of CAD...My understanding is that once ANY tool in the tool table is zeroed to the stock, any OTHER tool will have the correct reference because Mach, using the tool table, calculates the difference between the distance to the stock between the first tool that was zeroed and any other tool that gets called up- so why am I having this issue? here's a relevant portion of the g code if it would help:

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

Similar Threads:

• Fauna 21T tool offsets and work offsets
• How well do the factory probe routines work for simple work & tool offsets?
• Setting Tool and Work Offsets
• Best way to set work/tool offsets?
• Setting Work & Tool offsets

[CitizenOfDreams]

Here is what I think is happening with your setup.

You are zeroing your machine with tool #0, which I presume has the offset of 0 in your tool table - but the ACTUAL length of the tool you are zeroing with is about 3 inches.

Then you execute T12 M06 and apply the 3" offset from the tool table. So your Z coordinate is now -3", and the tool change macro needs to raise the spindle 3 inches to get back to 0. And you probably do not have 3 inches of travel left, so your Z axis bumps into the limit switch.

The easiest way to correct the problem would be entering the correct length of the reference tool in the tool table.

And yes, once ANY tool is zeroed, the rest of the tools will be right on the mark as well.

[tom.jelly]

I agree that that would be a logical thing to be wrong, but I do indeed have 3.6825 entered in the height field in the tool table. All of the numbers I have entered are positive, BTW which I think is what they are supposed to be..

[machinehop5]

TLOffsets are all most always is a negative number.

[CitizenOfDreams]

As I understand from your description, you zeroed the machine with tool #12 in the spindle. But what was the current tool in Mach3 at that moment? Was it #12, or was it still #0 by chance?

[tom.jelly]

The tool table is asking for "tool height" should I be entering negative numbers? How exactly does Mach 3 figure the tool offset? If I zero my tool 12, with a length from gauge line to cutting edge of 3.2" by touching off the stock and entering zero in the program run page works coordinates z field, what does Mach 3 look at to calculate its next z move? What about the next tool to be inserted?

[tom.jelly]

I know what you mean, that Mach 3 always starts from tool zero with zero tool length. Because I have tool 12 inserted and tool #12 showing in the program run tool information field before I even load the g code i'm 99% sure tool 12, but that is a good point that it may have switched to tool zero without me noticing it while loading the code. I'll have to check that tomorrow to be sure

[machinehop5]

should say Tool Height Compensation ...lol. Depending on the Programmer/Setup person if, positive or negative. if,you Set Z0 at the Top of Z travel (G28 Z0 Home) than all you have to do is load each Tool ...jog down to your Gage block of your choice above your Part and enter that number into offset.

[tom.jelly]

My g28 z0 home is indeed at the top of the spindle stroke. So I'll zero the part NOT machine coordinates DRO with the spindle located at MACHINE COORDINATE Z=0, then load tools 1 by 1, jog to the stock top and then enter the value shown in the PART coordinates DRO for each tool into the height field of the config>tooltable>height field, is this correct?

[machinehop5]

My g28 z0 home is indeed at the top of the spindle stroke. So I'll zero the part NOT machine coordinates DRO with the spindle located at MACHINE COORDINATE Z=0, then load tools 1 by 1, jog to the stock top and then enter the value shown in the PART coordinates DRO for each tool into the height field of the config>tooltable>height field, is this correct?

Yes,...to be on the safe side, dry run program with no tool in spindle.

PS- I'm not a Mach3 guy....but, that "Auto Tool Zero" button probably inserts the value of Z for you or maybe the "Remember" goood luck.

[Kenny Duval]

Be aware that Mach 3 has a known bug that was never fixed. You need to call the tool number in 1 line of code and then the tool offset in a separate line of code. If you call then in a single line Mach 3 will not apply the offset.

[tom.jelly]

This whole saga has been & will remain with the machine well clear of cutting anything until I know its working right

And it looks like the post I'm using calls the tool number Tx and then the offset, Hx in separate lines so I'm good there I hope...

[CitizenOfDreams]

Be aware that Mach 3 has a known bug that was never fixed. You need to call the tool number in 1 line of code and then the tool offset in a separate line of code. If you call then in a single line Mach 3 will not apply the offset.

Kenny, are you sure it has not been fixed? I am using version R3.043.062, and all my tool changes look like "T12 M6" (same line). The offsets are applied properly.

[Kenny Duval]

T12 M6 is just the tool change. You also need to call the tool offset which in your example would be H12. If this is called on a single line of code as

T12 M6 H12

then Mach will fail to apply the offset. It would need to look like the following.

T12 M6
H12

[CitizenOfDreams]

I see. Well, I have never used the H command, simple "T12 M6" applies the offset for me. Is a separate H command even necessary in Mach3?

[CitizenOfDreams]

P. S. Turns out my M6Start.m1s macro contains "G43.H" call (which applies the tool offset), but I do not remember whether I put it in myself or it was there from the factory.

[tom.jelly]

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)

[Kenny Duval]

Ok..so here is where I think you are going wrong. If the tool you referred to as your reference tool is being used to set your G54 offset then the offset for that tool should always be zero. It doesn't matter if you are setting up a part or setting tool offsets that particular tool should always have a zero length offset. Now when you are measuring tools you pick the surface you want to measure from, touch the reference tool to it and zero the Z DRO. Next switch to the tool you want to measure the offset for and jog it down to touch the same surface. Note the DRO measurement. That is the value that needs to be put in for that tools offset. If the tool is shorter than your reference tool then it will be a negative number. If the tool is longer than your reference tool then the number will be positive. This is how the machine tracks the relative difference between tools. Once you have measured the tool offsets then move to setting your G54 part zero datum with your reference tool in the spindle. There is also a setting in Mach 3 for setting the tool change safe Z and tool change position. Those need to be set before you run a tool change.

Have a look at the following video and it's other parts.



https://www.youtube.com/user/CVIMSM/...able_polymer=1

This is for the Mach Standard Mill add on but he does a great job of explaining offsets and how to measure them better than I think I can.

[machinehop5]

try this for the hell it.....put Z-1.200 in Offset 12...and see if your T12 runs correctly. The Master Tool ref thing....is want Big Shops use its very confusing and dangerous if, you change an Offset wrong.

[CitizenOfDreams]

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.