What's new
What's new

Tool heights and Z axis work offset

MRudisill

Plastic
Joined
Jan 13, 2020
I am missing something simple here...

I touched all the tools off to a common point on the table. I am then using my Haimer to measure from that point to the top of the workpiece and setting that value in the work Z offset. I am definitely missing something as it keeps giving me a Z over travel when I tell it to go above the part.

Does anyone have any ideas?

I normally touch each tool off to the piece, but now that we are running parts using 7+ tools. It's nice to just have a one tool touch off option.
 
Did you make your haimer a "tool" (like T99) and set a length offset for it? And call up that H offset when using it? Could be the issue.

Sent from my SM-N960U using Tapatalk
 
Yeah... my dumbass simply forgot the H43. Surprised the Haas didn't throw me an error for that like it does when there are a tool and tool height mismatch. Guess that's what I get for relying 99% on the software and not manually coding anything the last 6 months lol.
 
What happens if you set a tool to the top of the workpiece and then tell it to go above the part. Skipping the common point.

EDIT:
nevermind, the other posts didn't show up for me until I replied.
Weird.
 
Along the same lines, I was wondering if anyone knows how to simplify setting the z work offset.

All my tool lengths are set with a 2” gauge block off the table.
My current procedure is to pick any tool and touch it on the part top, then subtract the tool length offset from the machine z position. This is then manually entered into the z work offset. Im wondering if there is a way to simplify this so I don’t need a calculator or to manually enter the value. Too much room for operator error and its time consuming.

Can I use mdi to make the tool length offset active and use the operator coordinates? Whenever I put the machine in handle jog the position display seems to cancel all the active offsets.

Basically trying to get one of the coordinate readouts to display my position of tooltip relative to the 2” gauge block height (where all my tools are set to zero without any work shift)

Sorry if that was a poor explanation


Sent from my iPhone using Tapatalk
 
Standard procedure would be to chuck up an indicator, zero it on the 1-2-3 block then zero it on the work offset and use the position screen
 
Along the same lines, I was wondering if anyone knows how to simplify setting the z work offset.

All my tool lengths are set with a 2” gauge block off the table.
My current procedure is to pick any tool and touch it on the part top, then subtract the tool length offset from the machine z position. This is then manually entered into the z work offset. Im wondering if there is a way to simplify this so I don’t need a calculator or to manually enter the value. Too much room for operator error and its time consuming.

Can I use mdi to make the tool length offset active and use the operator coordinates? Whenever I put the machine in handle jog the position display seems to cancel all the active offsets.

Basically trying to get one of the coordinate readouts to display my position of tooltip relative to the 2” gauge block height (where all my tools are set to zero without any work shift)

Sorry if that was a poor explanation


Sent from my iPhone using Tapatalk

No control mentioned, but this works on Fanuc OMC and may be relevant to other models. With your tool in the/a measuring position and the cursor properly positioned in the tool offset tables at the tool number in question, you can hit EOB Z INPUT and it will place the current machine Z coordinate into your offset table. You hit the EOB Z buttons the same way you might do Control Alt Delete on a normal computer. The number will appear in the buffer area and then go into the table with INPUT.

If you want to take your measuring block into consideration, you can enter a positive Z value in your EXT offset and it will add that length to the number being input. I have a 4" height setter. I put Z4. in EXT and it gives me an offset that represents the distance as if I measured off the table. Just don't forget to change EXT Z back to 0 or your first tool will cut air. Using the EXT offset during tool height setting, you can lie to the computer any way you want to give you the numbers you're after without doing the math on a calculator and entering it in manually.

Simple Example. I have a fixture where program Z zero is -0.035 below the surface the setting device is able to sit on. I put Z4.035 in the EXT and it makes all my tool heights good without any math. Easy like that.
 
No control mentioned, but this works on Fanuc OMC and may be relevant to other models. With your tool in the/a measuring position and the cursor properly positioned in the tool offset tables at the tool number in question, you can hit EOB Z INPUT and it will place the current machine Z coordinate into your offset table. You hit the EOB Z buttons the same way you might do Control Alt Delete on a normal computer. The number will appear in the buffer area and then go into the table with INPUT.

If you want to take your measuring block into consideration, you can enter a positive Z value in your EXT offset and it will add that length to the number being input. I have a 4" height setter. I put Z4. in EXT and it gives me an offset that represents the distance as if I measured off the table. Just don't forget to change EXT Z back to 0 or your first tool will cut air. Using the EXT offset during tool height setting, you can lie to the computer any way you want to give you the numbers you're after without doing the math on a calculator and entering it in manually.

Simple Example. I have a fixture where program Z zero is -0.035 below the surface the setting device is able to sit on. I put Z4.035 in the EXT and it makes all my tool heights good without any math. Easy like that.

Should have clarified, HAAS control like the OP. Don’t think its the same as fanuc.


Sent from my iPhone using Tapatalk
 
Should have clarified, HAAS control like the OP. Don’t think its the same as fanuc.


Sent from my iPhone using Tapatalk

Ahh, I see that know. Yes doubtful, even on later Fanucs. I guess I'm inclined to share the knowledge. I went maybe 8 years on an OMC punching in numbers before I saw a guy do it on another OM. It was one of those - "what the fuh?" moments. Have punched in very few tool heights since. Stuff like that can happen when you always work alone.
 
Along the same lines, I was wondering if anyone knows how to simplify setting the z work offset.

On your Haas, go to Setting 64 - Tool Offset Measurement Uses Work Offset - and turn it OFF.
By doing this, you uncouple the tool offsets from the work offsets.

Then, jog each of your tools to a point somewhere on your table, I typically use a 2" gageblock on the fixed jaw.
When the block is touched, hit the Tool Offset Measur button.
Do this to all your tools.
Then, take an indicator ( Haimer is nice, but any dial indicator will do ) jog to the top of the 2" block and zero the Operator Z
Then move over to your part, jog down or up to your part 0, read the operator offset and enter the value in the workoffset field.
Done!

There is nothing to deduct, add, subtract, multiply, divide or even standing on left foot.
Done!

When adding more tools or replacing a broken one, just once again jog to the top of the 2" block, hit Tool Offset Measur and done.

Remember, with Setting 64 being OFF, the tool and work offsets become separated and instead of one driving the other, they will both be driven by the common 2" block instead.
 
seymourdumore,

All of my tools are touched off on a 2” block off the table at all times, and my setting 64 is off.
Your process makes sense, and I like the idea of using an indicator because there is nothing to crash, however it still requires a separate tool to be called up and touched off the gauge block.

I am specifically asking if there is a way to set the control so you can use any of the already zeroed tools to set the work offset. Frequently I will not set a single tool length offset for a particular job, so it is fastest to just call up a tool (say 1/2” endmill) and jog onto the top of the part. Then I subtract the tool offset from the current machine position to get my z offset. If the control could be put in handle jog mode with my tool offset active it would give me this work shift value in real time as the machine was jogged in Z.

Im going to play with it this afternoon, but it seems every time I switch into handle jog mode it cancels any active tool offsets.


Sent from my iPhone using Tapatalk
 
seymourdumore,

All of my tools are touched off on a 2” block off the table at all times, and my setting 64 is off.
Your process makes sense, and I like the idea of using an indicator because there is nothing to crash, however it still requires a separate tool to be called up and touched off the gauge block.

I am specifically asking if there is a way to set the control so you can use any of the already zeroed tools to set the work offset. Frequently I will not set a single tool length offset for a particular job, so it is fastest to just call up a tool (say 1/2” endmill) and jog onto the top of the part. Then I subtract the tool offset from the current machine position to get my z offset. If the control could be put in handle jog mode with my tool offset active it would give me this work shift value in real time as the machine was jogged in Z.

Im going to play with it this afternoon, but it seems every time I switch into handle jog mode it cancels any active tool offsets.


Sent from my iPhone using Tapatalk


You have macros on that thing?
 
If you had your tool offsets set to gauge length, then you could do what you're saying with just the part zero set button, but that would probably more annoying then just dealing with the offset unless your tools last forever.
 








 
Back
Top