Radius/Wear Comp on Haas Mill

[Mick]

I was talking to someone this morning that asked me a question, and I wasn't sure of the answer.

 

On the Haas mill control, there is a table for radius compensation, and wear radius compensation. It is my understand that when G41/G42 is applied, with the D value, that the radius and wear comp are added together and the coordinates shifted that combined amount.

 

My question is: Is there a separate g-code to apply just the wear amount?

 

The reason for this, is in the case of the user programming with just wear comp, and not wanting to zero the radius comp, as he has other programmes that use radius and wear comp combined.

[gcode]

just set the radius column to 0

[Mick]

just set the radius column to 0

 

That is what he considered doing, but he has some programmes that use full comp (and not wear).

 

I didn't think it was possible to call wear comp only. At least, with all the controls I've ever used, it isn't possible.

 

I suggested to him that he just needed to be diligent and set the radius column depending on the programme he was running.

[Mr. M]

Can he check the value in the radius column for the tools at the top of the program and fire a user alarm if it is not zero? Or just set them all to zero, but the first way alerts the operator so if he goes back to a program using it he isn't suprised.

[Machineguy]

No alarms will happen. Your operator need to pay attention and adjust those comps for every program.

Its good practice to zero all those tool comps out at the end of each program to be safe!!

Also it should be stated in the setup sheet that the values need to be based on how the program is written.

 

Machineguy

[jlw™]

Just wondering here, Haas doesn't support macro? If it does, dig on the manual and find the variable and call an alarm.

 

In a Mazak it would look similar to:

 

IF#55006EQ0.#3006=1(NO*COMP*VALUE)

 

Just curious but I imagine you can evaluate and alarm if needed.

[Machineguy]

If macros are turned on, yes that is a option.

[mkd]

 

The reason for this, is in the case of the user programming with just wear comp, and not wanting to zero the radius comp, as he has other programmes that use radius and wear comp combined.

I'd suggest a set standard in the shop. switching back and fourth is a good way to get everyone screwed up and confused...including the programmer.

 

that being said the program could have a G10 calls at the top to set the required offsets, which IMO, is probably the best way to eliminate confusion.

[Mick]

Thanks for all the replies everyone.

 

As mkd suggested, a standard in the shop is the best method. How this came about, was that the programmer had never used wear offset, but now having realised the benefits of it, wants to use it.

 

I did point out to him, that the cleanest, easiest way was to re-gen/re-post all toolpaths that were using radius comp to wear comp.

 

I do like the idea of a macro though. That could be a good fix.

 

I totally agree, switching back and forth will result in confusion.

[Newbeeee™]

I'd suggest a set standard in the shop. switching back and fourth is a good way to get everyone screwed up and confused...including the programmer.

 

that being said the program could have a G10 calls at the top to set the required offsets, which IMO, is probably the best way to eliminate confusion.

That's how we do it - prog automatically G10's the size into the machine control table, and then we tweak as required.

[mkd]

That's how we do it - prog automatically G10's the size into the machine control table, and then we tweak as required.

i have never implemented this in the post, but it sure sounds like a lifesaver. (i'm the one that forgets to adjust comps from the last job)

 

is it common to have the logic output G10 0.0 for wear comp and G10 .500" for a 1/2" EM using control comp?

[Newbeeee™]

Don't shoot me - we only use control comp or computer. We don't use wear (I like the sound of wear and have done for a couple of years but to change our shop with 10 years of historic progs would be suicide...)

So for a 10mm cutter, the G10 line will say R5.0 and dump that in the control overwriting whatever is on there so it's safe. The D column this is.

What it won't/can't do on loading into the control is to zero the related wear column and I can't see a parameter that can do this.

So in checking the tool table when setting tool lengths (H) we scan across to see if the Wear is 0 (talking fanuc here).

HTH

[taperlength]

To set the Wear Offset to zero for a tool number _n_

 

G10 L13 Pn R0

 

Just put that in a looping macro that increments the variable n, to set all the wear offsets to 0

[Newbeeee™]

To set the Wear Offset to zero for a tool number _n_

 

G10 L13 Pn R0

 

Just put that in a looping macro that increments the variable n, to set all the wear offsets to 0

Taper,

Excuse my ignorance but what do you mean?

Can you please supply a sample prog for a 24tool machine?

Thanks

[Colin Gilchrist]

Taper,

Excuse my ignorance but what do you mean?

Can you please supply a sample prog for a 24tool machine?

Thanks

 

 

Here is a sample with some comments for each line:

(FIRST, SET A VARIABLE TO ONE TO START THE LOOP.)
(COMMON VARIABLES ARE #100-#149 ON MOST "FANUC" STYLE CONTROLS)
#101 = 1

(SET LOOK AHEAD LIMIT TO 1 BLOCK, FOR HAAS CONTROLS!)
(YOU MAY NEED TO MODIFY THIS LINE FOR YOUR SPECIFIC CONTROL)
G103 P1

(START "WHILE" LOOP)
WHILE [#101 LE 24] DO 1

(SET TOOL WEAR OFFSET TO ZERO, USING LOOP COUNTER AS TOOL #)
N1 G10 L13 P#101 RO.

(INCREMENT LOOP COUNTER BY 1, TO RESET LOOP, AND INCREMENT T#)
#101 = #101 + 1

(LOOP ENDS WHEN CONDITION IS SATISFIED)
END 1

(CANCEL 1 BLOCK LOOK AHEAD LIMIT, FOR HAAS CONTROLS!)
(YOU MAY NEED TO MODIFY THIS LINE FOR YOUR SPECIFIC CONTROL)
G103 P0

Here is a sample without the comments for clarity:

#101 = 1
G103 P1
WHILE [#101 LE 24] DO 1
N1 G10 L13 P#101 RO.
#101 = #101 + 1
END 1
G103 P0

Hope that helps,

 

Colin

[Colin Gilchrist]

If you haven't already, look in this thread, and download all of the Macro B PDF files near the bottom of the page...

 

http://www.emastercam.com/board/topic/76926-cool-macros/page-4

[Colin Gilchrist]

The "Quick Reference" is especially handy. I printed out both pages and pinned them to my cube wall...