[mactec54]

[QUOTE=machinehop5;2404118]...I found an example of someones Hobbing program from cncmanuals. If you have a B axis you can make gears with it....if, not it's example of Mazatol format [QUOTE]

This has no relationship to what the OP is trying to do this example is controlled with a macro a completely different way to program, it was established early on that his control is not using Mazatrol format, not to say that it can't, it has to be in the Mazatrol mode if it has it

[mactec54]

[QUOTE=mactec54;2404136][QUOTE=machinehop5;2404118]...I found an example of someones Hobbing program from cncmanuals. If you have a B axis you can make gears with it....if, not it's example of Mazatol format [QUOTE]

I have to agree with what you are say though as it appears to be that they don't use the G43 in any of these older controls using the EIA code format, it also looks like it is good with using Macro's which would over come the low memory size the machine has so the OP has a lot to learn so he can program using Macro's

[machinehop5]

I have to agree with what you are say though as it appears to be that they don't use the G43 in any of these older controls using the EIA code format, it also looks like it is good with using Macro's which would over come the low memory size the machine has

...the G43 is there looks like but, no H for Tool offset.....I'm guessing the TxxM6 loads the geometry and H is confusing the control. He said would test this way later today.

[ashes-man]

I am pretty sure I have tried that. I definitely tried using T1M6 as well as H1. I have tried so many combinations I really cant remember. I will give it a go tomorrow and see what happens. From my understanding this machine does not have any relationship between tool selection and tool offset but I will try as only takes a few minutes.

I tried this again this morning with a tool selected and no H. It did the arc properly but without any tool offset. So adding a tool selection makes no change, but removing the H fixes the arc as it always has, but there is no tool offset.

[machinehop5]

I tried this again this morning with a tool selected and no H. It did the arc properly but without any tool offset. So adding a tool selection makes no change, but removing the H fixes the arc as it always has, but there is no tool offset.

...I see a few Params that affect the way Mazatrol handles T codes on this List below... not sure if its for your machine. look in your Service Manual if not

Attachment 449370

[ashes-man]

...I see a few Params that affect the way Mazatrol handles T codes on this List below... not sure if its for your machine. look in your Service Manual if not

Attachment 449370

Thanks, that manual is the service manual for my machine. My machine is a MAC-TP according to the startup screen, but appears to be identical to the IMAC-TP mentioned in that manual. I just checked and the IMAC-TP parameters aren't shown for those tool options. That may not mean they wont work though, maybe! I checked all parameters and they are as per the original printout from when the machine was built. This machine will do a tool change if you put just T1, no M6 required. It caused some grief as the fusion 360 post processor always pre-loads tools with a Tx after a tool change with TxM6. Even though you can turn pre loading off in the options it did it anyway. I had to edit the pre-processor to remove it!

What does "2 digits + 2 digits" mean for the T codes?

[machinehop5]

"What does "2 digits + 2 digits" mean for the T codes?" ..... That's for IMAC-LP looks like for Lathe maybe

[machinehop5]

...something doesn't make sense in this Test because if the Offset H2=125 than why is machine only going to Z-.75 when commanded to Z0

try using G44 maybe also,, try adding the Y's and J's dims , even if it's zero

Attachment 449398

[mactec54]

Thanks, that manual is the service manual for my machine. My machine is a MAC-TP according to the startup screen, but appears to be identical to the IMAC-TP mentioned in that manual. I just checked and the IMAC-TP parameters aren't shown for those tool options. That may not mean they wont work though, maybe! I checked all parameters and they are as per the original printout from when the machine was built. This machine will do a tool change if you put just T1, no M6 required. It caused some grief as the fusion 360 post processor always pre-loads tools with a Tx after a tool change with TxM6. Even though you can turn pre loading off in the options it did it anyway. I had to edit the pre-processor to remove it!

What does "2 digits + 2 digits" mean for the T codes?

Yes your control is reading the tool offset from the tool call # as you would of already set the tool to the top of your part that would be Z0 start point in your code

Any extra code you put in the program it won't know what it is, it may do something crazy or just stop, sometimes they will ignore the foreign code and just keep going

Try a T01 for tool call or any other tool number you are using, I see in your parameters that you can choose if you have 1 digit or 2 yours is most likely standard with 2 digits, a Tool call in true Code format is written as T01 different manufactures eliminated the need for the 0 as most controls it is not needed

Also in your test code remove the G49 in the safety line as that will cancel your tool offset

[ashes-man]

...something doesn't make sense in this Test because if the Offset H2=125 than why is machine only going to Z-.75 when commanded to Z0

try using G44 maybe also,, try adding the Y's and J's dims , even if it's zero

Attachment 449398

The G54 Z work offset is -200 (machine coord), the tool length is 125, so when the tip of the tool is at work Z zero, the machine Z coord is -200 + 125 = -75. So the spindle stops at Z-75 as the 125mm long tool reaches down to -200 where the top of the work is. Is this not right?

I did go and try G44 and reversing the tool offset length sign and got exactly the same behavior.

[ashes-man]

Yes your control is reading the tool offset from the tool call # as you would of already set the tool to the top of your part that would be Z0 start point in your code

Any extra code you put in the program it won't know what it is, it may do something crazy or just stop, sometimes they will ignore the foreign code and just keep going

Try a T01 for tool call or any other tool number you are using, I see in your parameters that you can choose if you have 1 digit or 2 yours is most likely standard with 2 digits, a Tool call in true Code format is written as T01 different manufactures eliminated the need for the 0 as most controls it is not needed

Also in your test code remove the G49 in the safety line as that will cancel your tool offset

My machine does not have the 2 digit tool code option. See a few posts back. But, I have tried with T1 and T01 and it seemed to be OK with both form memory. I will try again to be sure. I did some experiments swapping back and forth between tools (with different offsets set) and then going to G54 Z0. It always went to the same spindle location, not the same tool tip location. To my knowledge the machine doesn't relate tool numbers to offset numbers. There are 10 tools and 128 offset numbers.

But you could be right that the G49 is cancelling the tool offset. I have done tests with a tool change (T1 M6) after the G49 line. So that should restore the offset?

I will go back to the machine and do some more playing based on these suggestions though.

[ashes-man]

I will go back to the machine and do some more playing based on these suggestions though.

Tonight I set two tool length offsets H1=100mm, H2=50mm. I did T1M6;G0X0Y0Z0. Set a pointer at the tool tip. Did a T2M6; G0X0Y0Z0. The tool tip was 50mm above the pointer.

Then I did T1M6;G43H1;G0X0Y0Z0. Set the pointer to tool tip. Did T2M6; G43H2; G0X0Y0Z0. The tool tip landed exactly on the pointer. So, I think this proves the tool change does not set tool length offset.

I also reviewed the tool change macro and it does not call G43/44.

[machinehop5]

Tonight I set two tool length offsets H1=100mm, H2=50mm. I did T1M6;G0X0Y0Z0. Set a pointer at the tool tip. Did a T2M6; G0X0Y0Z0. The tool tip was 50mm above the pointer.

Then I did T1M6;G43H1;G0X0Y0Z0. Set the pointer to tool tip. Did T2M6; G43H2; G0X0Y0Z0. The tool tip landed exactly on the pointer. So, I think this proves the tool change does not set tool length offset.

I also reviewed the tool change macro and it does not call G43/44.

...looks like your test proves how the Tool Length Comp works....now I wonder if a Dxx code with a G42 or G41 Diameter Comp code is needed in G18 mode ZX move to fix the original problem

[mactec54]

My machine does not have the 2 digit tool code option. See a few posts back. But, I have tried with T1 and T01 and it seemed to be OK with both form memory. I will try again to be sure. I did some experiments swapping back and forth between tools (with different offsets set) and then going to G54 Z0. It always went to the same spindle location, not the same tool tip location. To my knowledge the machine doesn't relate tool numbers to offset numbers. There are 10 tools and 128 offset numbers.

But you could be right that the G49 is cancelling the tool offset. I have done tests with a tool change (T1 M6) after the G49 line. So that should restore the offset?

I will go back to the machine and do some more playing based on these suggestions though.

The G49 will still cancel the tool offset it is best to remove it, it should never be in the safety line, if you had a need to use a G49, it should only be used after the G43, if you think you need it, which in most cases it is never needed

G49 is a G-code that helps in the cancelation of both G43 and G44 tool length compensation. If you use the offset amount as H00, it can also scrap the tool length compensation.

Good that you have found that the standard tool change T-- M6 works so apart form getting the offset sorted you should be able to use standard Fanuc format code

[ashes-man]

...looks like your test proves how the Tool Length Comp works....now I wonder if a Dxx code with a G42 or G41 Diameter Comp code is needed in G18 mode ZX move to fix the original problem

I guess there is no harm trying. I have not tried any cutter diameter compensation yet...

[ashes-man]

The G49 will still cancel the tool offset it is best to remove it, it should never be in the safety line, if you had a need to use a G49, it should only be used after the G43, if you think you need it, which in most cases it is never needed

G49 is a G-code that helps in the cancelation of both G43 and G44 tool length compensation. If you use the offset amount as H00, it can also scrap the tool length compensation.

Good that you have found that the standard tool change T-- M6 works so apart form getting the offset sorted you should be able to use standard Fanuc format code

The tool change macro has a G49 after the tool is placed back in the rack. However, it does not do a G43/44 after it gets a new tool out.

T1, T01, T1M6 and T01M6 all cause the tool change macro to be run.

[mactec54]

The tool change macro has a G49 after the tool is placed back in the rack. However, it does not do a G43/44 after it gets a new tool out.

T1, T01, T1M6 and T01M6 all cause the tool change macro to be run.

That is fine to have the macro to do that, that is another good reason not to have it in your program anywhere

So that is what you have to determined if you need to use the G43 or not, or just the T1M6, forget about the G44 it is another one of those codes that are rarely ever used in normal programing and can easy cause a crash if used incorrectly

[ashes-man]

So that is what you have to determined if you need to use the G43 or not, or just the T1M6, forget about the G44 it is another one of those codes that are rarely ever used in normal programing and can easy cause a crash if used incorrectly

From what I can see I have no choice but to use G43 in my code as no other way to get tool length compensation. I could have no G43 and do all the length compensation in cam but that would not be ideal as I would need to know exact lengths before post processing every time. If I didn't use G43 then everything would just work though as far as the XZ/YZ arcs! The fusion 360 Mazak post processor generates G43 for the first Z move after each tool change.

[machinehop5]

I guess there is no harm trying. I have not tried any cutter diameter compensation yet...

... your machine has which type on Tool Comp format A B or C ?

I was reading this thread and Mazatrol is about the same format ....I think 25 years ago..may help
https://www.cnczone.com/forums/fanuc...ation-b-c.html

thx gentlegiant

plugin from cncmanuals...
Download PDF Fanuc 16 18-B Machining Center Operator Manual - CNC Manual
15.1 page 247 or so

[ashes-man]

... your machine has which type on Tool Comp format A B or C ?

I was reading this thread and Mazatrol is about the same format ....I think 25 years ago..may help
https://www.cnczone.com/forums/fanuc...ation-b-c.html

thx gentlegiant

plugin from cncmanuals...
Download PDF Fanuc 16 18-B Machining Center Operator Manual - CNC Manual
15.1 page 247 or so

Thanks. I am guessing from the description in that thread and manual, my machine has type C. It has four columns; length, length wear, diameter, diameter wear. That manual is about the most easy to understand one I have seen. The Mazak ones seem to be written in Jinglish (excuse the term!).