[Deano7/11]

Ok after reading the manual plenty of times and reading heaps on the net I still have questions about the use on g50 in the work offset
I get that the g50 x.. Z.. Are the distance from the work piece zero to the tool tip but how does the following work

Lets say I have a rougher turning tool in pos 1 and the g50 is x150 z 200 and the stock 0 is the front of the stock.
This particular op take 3 tools how does things when I do a tool change ? Is the offset amount stored in the control just the difference between the 3 tools and say tool 1 will be a master tool that I always use to set work zero?

So if the g50 is always x150 z200 but in the offsets I have the following
tool 1 as x0 z0 (master tool)
Tool 2 as x10 z5(finisher tool with 10mm more stick out in x and 5 more in z)
Tool 3 x -150 z10 (centerline tool like drill bit)

Am I even on the correct path with this set up?

[angelw]

Ok after reading the manual plenty of times and reading heaps on the net I still have questions about the use on g50 in the work offset
I get that the g50 x.. Z.. Are the distance from the work piece zero to the tool tip but how does the following work

Lets say I have a rougher turning tool in pos 1 and the g50 is x150 z 200 and the stock 0 is the front of the stock.
This particular op take 3 tools how does things when I do a tool change ? Is the offset amount stored in the control just the difference between the 3 tools and say tool 1 will be a master tool that I always use to set work zero?

So if the g50 is always x150 z200 but in the offsets I have the following
tool 1 as x0 z0 (master tool)
Tool 2 as x10 z5(finisher tool with 10mm more stick out in x and 5 more in z)
Tool 3 x -150 z10 (centerline tool like drill bit)

Am I even on the correct path with this set up?

Each tool has a separate X and Z G50, with the offsets designed to be used as Wear Offsets. Following is an example using the differences shown in your above three tools.

O0001
(OD T/TOOL - ROUGH FACE AND OD)
N1 G21 G40 G99
G28 U0.0 W0.0
G50 X150.0 Z200.0
G50 T0100 S3000
G96 S250 M03
G00 X_ Z10.0 T0101 M08
----------
----------
----------
G00 X150.0 Z200.0 T0100 M09
M01
(OD T/TOOL - FINISH FACE AND OD)
N2 G28 U0.0 W0.0
G50 X140.0 Z195.0
G50 T0200 S3000
G96 S250 M03
G00 X_ Z10.0 T0202 M08
----------
----------
----------
G00 X140.0 Z195.0 T0200 M09
M01
(DIA 20.0 U/DRILL - ROUGH DRILL FOR B/BAR)
N3 G28 U0.0 W0.0
G50 X300.0 Z190.0
T0300
G97 S3000 M03
G00 X0.0 Z10.0 T0303 M08
----------
----------
----------
G00 X300.0 Z190.0 T0300 M09
M05
M30
%

If you call the tool offset with the tool call out, you will observe the X and Z slides move by the values stored in the respective Tool Offsets. Accordingly, its good practice to apply the Tool Offset with the first move command, where in doing so the offset is seamlessly applied and unseen. Its also important that the tool offset be cancelled when the tool is returned to the Tool Change point. G50 coordinate set should be applied with the slides parked at the same location exactly, for each individual tool. As the Reference Return position is the easiest location to repeatedly find, that location is often used to apply the G50 coordinates. This may not be practical with a machine that has a considerable Z axis travel. To make a closer Z location to use as a Tool Change position, an incremental move from the Reference Return position can be used.

Regards,

Bill

[Deano7/11]

thanks for the great reply Bill

the way you explain the offsets makes sense as the machine had very small values in the offsets eg .005, .010 etc,

so are my G50 values are stored outside the control and inserted into the code when writing the code based on the tool used and the stock zero position?

if this is the case i assume i would keep a external record of the g50 values for each tool and then when writing the code i would look up my g50 list for each tool and insert accordingly?

if this is correct can i record the g50 value based on a common part of the machine eg chuck face and then adjust the g50 prior to inserting into the code by the difference between the chuck face and stock zero? so based on the examples below if the stock was now 20mm further forward than the 200 (tool 1) my g50 will be adjusted to g50 x150 z180 and the rest of the tools will be adjusted by the same 20mm difference?

i would suspect if the above is correct that the only real value that will change as the stock zero changes is the Z value as X is alway the spindle centre line?

[angelw]

thanks for the great reply Bill

the way you explain the offsets makes sense as the machine had very small values in the offsets eg .005, .010 etc,

so are my G50 values are stored outside the control and inserted into the code when writing the code based on the tool used and the stock zero position?

if this is the case i assume i would keep a external record of the g50 values for each tool and then when writing the code i would look up my g50 list for each tool and insert accordingly?

if this is correct can i record the g50 value based on a common part of the machine eg chuck face and then adjust the g50 prior to inserting into the code by the difference between the chuck face and stock zero? so based on the examples below if the stock was now 20mm further forward than the 200 (tool 1) my g50 will be adjusted to g50 x150 z180 and the rest of the tools will be adjusted by the same 20mm difference?

i would suspect if the above is correct that the only real value that will change as the stock zero changes is the Z value as X is alway the spindle centre line?

Yes, all your assumptions are correct.

By referring to predetermined dimensions from, say:
a. Turret Face to Chuck Face
b. Boring Bar holder centre line to Spindle centre line.
c. Turret Side Face to Boring Bar centre line.

G50's for X and Z can be obtained by measurement of the tool and workpiece protrusion from the respective datum surfaces. By keeping good record of the dimensions in "a" to "c" above, that can be referred to, G50's for use in the program can be calculated away from the machine if the program is being prepared on a PC in a remote location.

The exact G50 for X and Z is obtained at the machine by touching off the tool on known dimensions of a blank work piece, say Z0.5 and X50.0 if after taking a cleanup cut on the end and diameter respectively, result in those actual dimension. Because an integer value in the metric system is relatively small (1mm = 0.0394"), I use the integer component of the exact distance from the component X, Z Zero to the point where the G50 is applied, as the G50 value in the program, and the remaining decimal part is registered in the Tool Offset.

Lets say the the X,Z Reference Return position is to be used as the Tool Change location. In that case I would do the following to obtain the exact G50.

1. Perform a Reference Return for both the X and Z axis and Zero the display of each axis on the Relative Position Page.
2. Manually Select the tool to set, and with a blank workpiece mounted in the work holding device, start the spindle.
3. Move the tool manually to the workpiece and take a cleanup cut on the face.
4. Move the tool clear of the workpiece in X without moving the tool in Z.
5. Stop the spindle and by measurement, determine how much material is left between the machined face and Z zero of the workpiece.
6. The Z display will be showing a distance from the Z Reference Return Position to the current Z position of the tool, in a minus direction.
7. Disregard the minus sign of the displayed Z value and add the material left on the workpiece face to this number.
8. The result of 7 is the exact G50 for that tool. Lets say that the result without the minus sign is Z200.672. I would use 200.0 as the G50 and register -.672 in the Z Offset for that tool.
9. Repeat from 3 to 8 above but replacing Z with X and taking a cleanup cut on the diameter before moving the tool clear of the workpiece in Z without moving the tool in the X axis. The value added to the current X value from the X Reference Return position will be the measured diameter of the cleanup cut made on the diameter of the workpiece.
10. Repeat from 2 to 9 inclusive for all tools to be set.

Regards,

Bill

[Deano7/11]

Bill

Thanks for taking the time to explain in such detail, it is all becoming more clear now.

I will have a look further tonight based on your explaination.

My machine has small travels so tool change will be done at machine home (zero retrun)

I notice you are in Australia, where abouts?

The plan is to use mastercam to generate the code. I am assume that the G50 values will have to be inserted manually after the code is output but before transferring to the CNC.

[angelw]

Bill

Thanks for taking the time to explain in such detail, it is all becoming more clear now.

I will have a look further tonight based on your explaination.

I notice you are in Australia, where abouts?

The plan is to use mastercam to generate the code. I am assume that the G50 values will have to be inserted manually after the code is output but before transferring to the CNC.

Deano,
With regards to the output via Mastercam, it depend on how well you organize your tooling information and machine datum dimensions. Mastercam has a tool library and tools can also be created on the fly if not a regular tool stored in the library. Accordingly, there's no reason why Mastercam couldn't output a file with the correct G50's in place, but it will require a fair amount of effort to get it all set up. It would be important that a setup sheet accompanied the program to the machine to ensure the operator set the tools with the correct amount of protrusion.

I live in Ballarat, Victoria. About 150km west of Melbourne.

Regards,

Bill

[Deano7/11]

thanks again Bill

currently mastercam outputs the following. not sure if this is good enough for the 6t. what do you think?
i know the spot where tool offset is applied is not ideal but unsure where or how to change that in the post.

also the post must get the g50 value from somewhere but stuffed if i can see it.

N100 G21
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 08)
N110 G28 U0. W0.
N120 G50 X250. Z250.
N130 G0 T0101
N140 G97 S2500 M03
N150 G0 X11.918 Z17.388
N160 G50 S2500
N170 G96 S120
N180 G99 G1 Z15.388 F.25
N190 Z1.919
N200 X13.864
N210 X16.692 Z3.333
N220 G0 Z17.388
N230 X9.972
N240 G1 Z15.388
N250 Z10.314
N260 X10.842 Z9.668
N270 G3 X11.183 Z9.11 R1.
N280 G1 Z1.919
N290 X12.318
N300 X15.147 Z3.333
N310 G0 Z17.388
N320 X8.026
N330 G1 Z15.388
N340 Z11.761
N350 X10.372 Z10.017
N360 X13.201 Z11.431
N370 G0 X14.364
N380 G28 U0. W0. M05
N390 T0100
N400 M01
(TOOL - 21 OFFSET - 21)
(OD FINISH RIGHT - 35 DEG. INSERT - VNMG 16 04 08)
N410 G28 U0. W0.
N420 G50 X250. Z250.
N430 G0 T2121
N440 G97 S3000 M03
N450 G0 X-.103 Z14.888
N460 G50 S3000
N470 G96 S120
N480 G1 Z12.888 F.5
N490 X5.178
N500 G3 X6.505 Z12.534 R.8
N510 G1 X10.51 Z9.556
N520 G3 X10.783 Z9.11 R.8
N530 G1 Z1.719
N540 X13.864
N550 X16.692 Z3.133
N560 G28 U0. W0. M05
N570 T2100
N580 M30
%

i am in Melbourne, down Frankston way, heading through Ballarat tomorrow as heading back to the folks in horsham for fathers day.

[angelw]

N100 G21
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 08)
N110 G28 U0. W0.
N120 G50 X250. Z250.
N130 G0 T0101
N140 G97 S2500 M03
N150 G0 X11.918 Z17.388
N160 G50 S2500
N170 G96 S120
N180 G99 G1 Z15.388 F.25

N380 G28 U0. W0. M05
N390 T0100
N400 M01


i am in Melbourne, down Frankston way, heading through Ballarat tomorrow as heading back to the folks in horsham for fathers day.

Its not too difficult to change the MasterCam Post, and I would definitely do that so that the Tool Change occurred without the Offset being called until the first move block. Also, its a good idea to cancel the Tool Offset on the move to Reference Return and not after it reaches there. You will see in the example code I listed earlier that I include G28 U0.0 W0.0 at the start of each new tool, and before executing the G50 Coordinate Set block, but I return the tool to home by specifying the coordinates of the previously specified X Z G50, and cancel the offset in this block.

The effect of G28 differs somewhat through various control models, but its my experience that the offset is cancelled as the tool travels to the Intermediate Point. When using the G28 command with Incremental values of Zero for X and Z by executing G28 U0 W0, the slides still return home via the Intermediate Point of Zero distance from the tool's current location. If the Offset did cancel during that Intermediate zero distance, you may see an unexpected move as the Offset cancels.

If the Tool Offsets don't cancel during the G28 move, and I've seen that situation as well, then when the Offsets are cancelled on the next block after the G28 U0 W0, the slides will move away from the Reference Return Position. The G28 block for the next tool would then move the slides back to the correct position before the G50 for the tool is executed, thus making things correct again. With the program arranged in the method shown above for returning the slides to home, you may observe some unnecessary shuffling of the tool between returning home and calling the next tool.

Apart from the above criticisms, the rest of the code output is workable.

I get down your way frequently. I do a lot of contract programming, CNC methodology, and automation projects.

Regards,

Bill

[Deano7/11]

Bill

sounds like i am on the right track at least with the post i have .

any ideas where in the post the offsets are and the way they are input into the code so i can make the changes that you mentioned

[Deano7/11]

I have now worked out where mastercam gets the G50 values from and they can be set in the tool so as a new tool is called the new G50 value will be inserted into the file.

i guess the trick would be to remember to change this to the correct z value before posting. or just make all z 0.0mm so if it is posted after forgetting to put in the correct z g50 value then it wont crash and when looking through the post prior to running i should notice a g50 with a z0 value.

[angelw]

I have now worked out where mastercam gets the G50 values from and they can be set in the tool so as a new tool is called the new G50 value will be inserted into the file.

i guess the trick would be to remember to change this to the correct z value before posting. or just make all z 0.0mm so if it is posted after forgetting to put in the correct z g50 value then it wont crash and when looking through the post prior to running i should notice a g50 with a z0 value.

Hi Deano,
Irrespective of how careful you are, if you try hard enough you can always set up a scenario to crash a CNC machine. MasterCam can be configured to output a close to perfect program for your needs, but it requires attention to detail. The trick is to have Z G50 for tools set in the Tool Library referenced to a constant Z component of the machine in the same way the X G50 is (centre line of the machine). The Chuck Face for this would be a good candidate. When the Job Setup is made in MasterCam, the Post Processor uses this information in conjunction with the data from the Tool Library to output the correct Z G50; but how accurate this is, comes down to how well you maintain the Tool Library and the values used in the Job Setup.

Many leave setting the G50 vales in the program to the machine operator, and purposely have the G50's in the program as recognizable wrong values, like the 0.0 value you suggested. However, if you were to run a program with G50 Z0.0 from the Reference Return position, its likely that the Z Slide will be driven into Hard Over-travel. If your standard approach to the Workpiece in Z is, say, Z5.0 or Z10.0, then it would be better to use a Z value of, say, 10.0. In this way, with the Z G50 set to 10.0, there will be no, or minimal movement of the slide, and Over-travel will be avoided.

Regards,

Bill

[Deano7/11]

Bill

I think I may have just had a light bulb moment so bare with me

as you have mentioned the g50 is the distance from the work x.z zero point to the home/t/c
i can set the home position as discussed via the tool table in m/cam and this value outputs in the post as the g50 position.
when the g50 line is called the machine cord change to the work cord so instead of being at home x0 z0 it is then in the g50 values from the work zero so what is z0 x0 (home/tool change pos) now becomes (as example) g50 z150 x200 so after this line in the code everything is then referenced to the work zero.

so once i set up my tool offsets into mastercam as my home position then i shouldn't have to change them. even the z value should be right on.

what has thrown me previous is the fact i had in my mind that the first move was the the actual g50 position but after looking at the code the first move is not the g50 values but just a rapid move to make the first cut.

here is 2 examples .

the same part in both but the first one has work zero at the back of the part and the second at the front of the part.

the g50 is correct for both but the first example has its z values in positive and the second in the negitive.

work zero at the back of the part
G21
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 08)
G28U0.W0.
G50X150.Z150.
G0T0101
G97S3600M03
G0X12.891Z17.388
G50S3600
G96S275
G99G1Z15.388F.25
Z1.919
X13.864
X16.692Z3.333
G0Z17.388
X11.918
G1Z15.388
Z1.919
X13.291
X16.119Z3.333
G0Z17.388

work zero at the front of the part.
G21
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 08)
G28U0.W0.
G50X150.Z150.
G0T0101
G97S3600M03
G0X12.994Z4.5
G50S3600
G96S275
G99G1Z2.5F.25
Z-10.968
X13.967
X16.795Z-9.554
G0Z4.5
X12.021
G1Z2.5
Z-10.968
X13.394
X16.222Z-9.554
G0Z4.5
X11.048
G1Z2.5
Z-3.306

so if i understand this right i could just reference all my z offests to the chuck face and pretty much call most of my work zero as the chuck face or offest the z value from home to the chuck face by the distance away from the chuck face if for the example i want to use the front of the stock as the zero point, so if the stock is 50mm from the chuck face i can either adjust my m/cam files or put the 50mm in the z offset

please correct me if i am wrong mate.

[angelw]

Hi Dean,
What you have said in your post is correct, but you can have the MasterCam Post processor calculate a Z G50 based on the Z value stored in the Tool Library and the Workpiece length.

If the chuck face is used as Z Zero, then, like the centre line of the machine for X Zero, the Z G50 for a particular tool won't change from job to job. However, even though the chuck end of the part is used for Z Zero, it still may not be the chuck face, it may be a step in soft jaws that will contact Z Zero, and the G50, or the Tool Offset will have to be offset by the distance from step to chuck face.

Tool Offsets with the Series 6T control were meant to be wear offsets, with the values being relatively small. It may be machine builder specific, but I've never seen a Series 6T where the slides didn't move by the amount registered for the respective tool offset when the offset was called without a move command. Accordingly, if you had a 50.00mm Z offset, the Z slide will move 50.00 in Z during the Tool Index. You can test this on your machine by parking the slides well away from any interference should the slides move during a tool index and offset call up, and execute a command to call a tool and offset with an offset of say 10mm or 20mm registered for the respective tool. If the slides move during the tool index, you need to be aware of this when using large offsets and when calling a tool and offset as shown in your listed program. You can conduct this test either using MDI or a command in a simple, memory registered program. Make sure you program G00 in the same line as the tool call command as follows, so that the slides can move.

G00 T0101

One hazard when using the chuck end of the workpiece as Z Zero, is that should you inadvertently input a Z move command without a decimal point in the coordinate, there exists a high probability of a devastating crash. Lets say:
1. the workpiece is being held in jaws that protrude from the chuck face by 45.0mm

2. that the chuck face is Z Zero.

3. the workpiece is 50.0 diameter and 100.00 long

4. your approach move to the workpiece is X52. Z105.

4 above will place the tool outside the diameter of the part and clear of the end by 5.0mm; everything is fine. During the run of the parts, an edit was made and Z105. was inadvertently input as Z105 (no decimal point). Z105 will be interpreted as Z0.105, and that will be 0.105 off of the face of the chuck, well and truly engaged with the chuck jaws. Conversely, if the tail stock end of the part is Z Zero, and the same error during editing is made, Z5.0 will be interpreted as Z0.005. This event won’t cause a crash if the tool is outside the diameter of the work, and if it weren’t, there would be contact with the end of the work if a machining allowance existed, but nowhere near as devastating as hitting chuck jaws.

Using a relatively large value in the Tool Offset to compensate for the length of the workpiece, still requires you to register the value in the tool offset for every tool being used. As these values will be large, there is a higher potential for a crash than if wear size (usually less than 1mm) offset values are used.

Regards,

Bill

[Deano7/11]

Bill

I understand what you mean about getting mastercam to output the correct g50 but without knowing how to do that I am a bit stuffed with that one so I guess manually inputting the x and z g50 values into the program prior to post processing seems like my only option. If I have the default z,x zero values as the chuck face then I would just then have to modify the value in z by the difference between the face of the chuck and the work zero.

I understand what you say about crashing and like you have mentioned if you try hard enough you can crash the machine.

So just to clarify I need the machine, relative and absolute cord to be 0,0 when I first do a zero return upon start up and the g50 will then take care of the work cord?

I have tried to run a program that is in the machine but if just give error 059, something about ‘not found in memory’
Must to doing something basic wrong

[angelw]

Bill

I understand what you mean about getting mastercam to output the correct g50 but without knowing how to do that I am a bit stuffed with that one so I guess manually inputting the x and z g50 values into the program prior to post processing seems like my only option. If I have the default z,x zero values as the chuck face then I would just then have to modify the value in z by the difference between the face of the chuck and the work zero.

I understand what you say about crashing and like you have mentioned if you try hard enough you can crash the machine.

So just to clarify I need the machine, relative and absolute cord to be 0,0 when I first do a zero return upon start up and the g50 will then take care of the work cord?

I have tried to run a program that is in the machine but if just give error 059, something about ‘not found in memory’
Must to doing something basic wrong

Hi Dean,
Once the tool's X G50 is set correctly in the MasterCam Tool Library you can use this value in your program, as the X0.0 doesn't change from job to job; its always the centre line of the machine.

When determining the G50 at the machine, the easiest method is to Reference Return the slides in X, Z and then Zero the Relative Display for both axis. When you touch off the tool on the workpiece, you only have to add to the current absolute value of the Relative Readout, the dimension of the material between the tool and X,Z Zero of the workpiece. You can do the same with all other tool requiring to be set without having to do another Reference Return and display Zero. You don't need to concern yourself with the Absolute Display. The Absolute Display can't be easily Zeroed as can the Relative Display. To change the Absolute Display, you have to do so by executing a G50 command.

Regards,

Bill

[bertus.nl]

Hi,

I think you must NOT use G50 and X...Z...,and use it only for setting max rpm.
because you have to do strange calculations from the machine zero(G28U0.W0.)
point. and i can not see why .
just use normal geometrical offset ,and normal workoffset G54 .

les think and type work.

vr gr bertus

[angelw]

Hi,

I think you must NOT use G50 and X...Z...,and use it only for setting max rpm.
because you have to do strange calculations from the machine zero(G28U0.W0.)
point. and i can not see why .
just use normal geometrical offset ,and normal workoffset G54 .

les think and type work.

vr gr bertus

The Series 6T control doesn't have Geometry Offsets. G50 is used to set the Coordinate System and to clamp the maximum spindle revs in Constant Surface Speed Mode.

Regards,

Bill

[bertus.nl]

hi,

strange i had a 3t (bj+/-1985) 6t and 10tf and all had ofsets .

see ofset button on pictureAttachment 202724

i think i have pictures of programs ad work ,i wil look on monday

vr gr bertus

[angelw]

hi,

strange i had a 3t (bj+/-1985) 6t and 10tf and all had ofsets .

see ofset button on pictureAttachment 202724

i think i have pictures of programs ad work ,i wil look on monday

vr gr bertus

Series 10T had Geometry Offsets, but not 6T, not even the the 6TB model. The Series 6 had offsets, but they were designed to be used as Wear Offsets with the coordinate system for each tool being set via G50. Work Shift Offsets were introduced with the 6MB control. The 6MA control used G92 to set the Coordinate System.

Regards,

Bill