Hi BR549
Tried you idea. Tool1 was the reference tool. I have that as a positive tool length.
Changed Tool 2 which is the first tool that actually cuts the part to a negative number.
The tool did not go to the correct position and starting drilling at the corner reference
of the part. Thnaks for the help. Still it seems I`m lost.

Barry, that's the one. It all seems correct, but i think your problem is you are using two length offsets.

One is in the tool table and one is on the line

G17 G20 G40 G54 G64 G90 G43

(Spot Bearing Center Using 11/32 Drill Tool2)

T2 M6

G43H2

(0.34375)

H2 is adding another 2" to the offset

I use this format at the beginning of a toolchange

N160 M08
N170 M03
N180 G43 H0 D0

At the end of using that tool i have a G49 to cancel the tool offset

Then i enable it again on the next toolchange

Easy with cam and a working post processor.

I suggest you try the tools manually to make sure the offests are in the correct format as follows

Set tool one in machine zero on a foam/sponge block (Something soft)

Enable tool offset

Change to tool two MOVE Z to zero it should in the correct position as i cant remember if the tools should be neg or positive numbers in the tool table as i am not at the machine and haven't used it for some time.

Repeat/check all other tools.

Your master tool should be Zero length then reference all other tools against it. THEN set the top of material to the master.

 I alway use the longest tool for the job as the master that assures all comp moves will be down not up. So you should never trip the upper limit.

OR the other method is to always measure against a master (longest tool length you ever use) and then set the top of material to the master before you begin. But with limited quill travel you can run out of travel(Knee mill)

Just a thought, (;-) TP

Using the tormach method the reference tool is my longest tool. The value in the tool table is a + value 5.2776.
It is not a zero length tool like some of the other methods use. I`ll take a guess and say that the tormach method
requires a long travel z. My machine is shorter then the z travel of a Tormach cnc. So BR549, with my limited knowledge
on such things I agree with your post.

THis may make it a little easier to read the code. I would set tool#2 =0.000 and then remeasure the rest of the tools. Then apply the offset for each tool in the tool table

T2=0.000
T3= x.*********
T4= X.*********
T5=X.*********

Then setup the program install tool#2 and touch off on the top of material and reset Z=0.000.

Now raise the tool up to a clearance height and start the program.

This assumes you do your tool changes away from the work area AND allow clearances to allow the machine to recycle the tool offsets after the tool change is complete and before it get back to the work.

Tool offsets can be done several different ways this seems to be an easy way.


*************************************************************

( Insert Tool#2 and set Z zero at Top of Material )

G17 G20 G40 G54 G64 G90 G49
G0 X0.0 Y0.0 Z1.000

(Spot Bearing Center INSERT 11/32 Drill Tool # 2 )
(0.34375)
G0 X-0.8000 Y1.3750 Z0.2000
G81 X-0.8000 Y1.3750 Z-0.1 R0.2 F105.0
G80

(Spot All Holes On Face Using 11/32 Drill Tool # 2)
G0 X-1.2336 Y0.7082 F100.0
G81 X-1.2336 Y0.7082 Z-0.1332 R0.2 F105.0
 X-0.8000 Y0.4000 Z-0.1332
 X-0.3664 Y0.7082 Z-0.1332
 X-0.3664 Y2.0418 Z-0.1332
 X-0.8000 Y2.3500 Z-0.1332
 X-1.2336 Y2.0418 Z-0.1332
G80

(11/32 Drill Mounting and Bearing Tool # 2)
G0 X-0.8000 Y2.3500
G83 X-0.8000 Y2.3500 Z-1.2 R0.2 F105.0 Q0.2
 X-0.8000 Y0.4000 Z-1.2
 X-0.8000 Y1.3750 Z-1.2
G80

(Drill 5/32 for 10-24 Bolt Tool # 3)
T3 M6
G43H3
(0.15)
G0 X-1.2336 Y0.7082
G83 X-1.2336 Y0.7082 Z-0.7 R0.2 F105.0 Q0.2
 X-0.3664 Y0.7082 Z-0.7
 X-0.3664 Y2.0418 Z-0.7
 X-1.2336 Y2.0418 Z-0.7
G80

(DrillTool 1.00 V End Mill Tool # 4)
T4 M6
G43H4
(0.875)
X-0.8000 Y1.3750 F8.0
G83 X-0.8000 Y1.3750 Z-1.5026 R0.2 F103.0 Q0.1
G80
G0 Z0.2000

(Step Drill Custom Bit Bearing Hole Tool # 5)
T5 M6
G43H5
(0.9)
G83 X-0.8000 Y1.3750 Z-1.25 R0.2 F103.0 Q0.1
G80
G0 Z2.000
G49
M05
M30
%


Hope that helps, (;-) TP

Hi BR549
I`m a bit unclear as to measuring the tools. Do I measure the overall tool length. Or would I determine the difference in
length from one tool to another. Then enter those values in the Mach3 tool table.
PS... Your time and effort with my issue is much appreciated. !!!!

Yes you measure the DIFFERENCE between the master tool and all the rest .  touch off the master tool to your reference surface. Set Z to zero. Then touch off each tool and look at the Z value. That number will be the tool offset. Change tool touch off record the number, until you run out of tools.

That will be the offset for each tool as compared to the master. ALSO remember that you set the TOM of the JOB to zero from the "master tool".

OOPS also you need to reset the FEERATES (;-) I had them running FAST to test the sequencing.

My time is your time until you get an understanding of the process, (;-)  TP

Hi BR549
I`m excited to get to the shop today and do testing. You`vie provided comprehensive
information here. I hope what`s left of my mind can comprehend the steps. I`ll provide
a report ASAP.
Thanks and Regards Barry

Hi BR549

Thanks to you my project is a success. With your code modifications and excellent
description of all the steps. I have a good understanding of what`s required.
Much Appreciated. You saved the day!!!!!

Barry

Barry I am glad you got it working,  I love it when a plan comes together and chips can start flyin.

(;-) TP