What's new
What's new

Fixed tool offset comp

GiroDyno

Hot Rolled
Joined
Apr 19, 2021
Location
PNW
We have 4 Haas VFs ranging from 2007-2012 running high volumes of the same parts year after year. We don't use the tool setting probe on our machines because they don't fit into our fixturing, instead we touch off by rolling a 1/2" EM under the tool tip, against the top of fixture. Once the EM rolls under the tool tip hit Tool Offset Measure, and adjust length wear by 4.0 (3.5" Fixture Height + 0.5" EM). Is there a way to automatically comp, or add that wear value? The fixture and endmill never change, so it's really just an opportunity for an operator to fat-finger a wrong decimal and blow something up.
I use one of those 2" tall light up tool setters on my Brother and I was able to set that 2" value in a parameter and the machine automatically comped for that whenever I'd set a tool, hoping the Haas can do the same...
 
You could set the Z for the top of the fixture plus 4.0 in an unused WCS, say G120. MDI G120, cycle start, then touch off the way you are currently.
 
Not quite what I'm looking to accomplish, but I thanks for the suggestion
That's still the same number of keystrokes (6) = same number of possible errors.
I'd like to save that number somewhere and have it automatically applied
Maybe I could alias the tool change macro like...

Code:
O9006 (SET COMP ON TC)
#1= -4.5 (COMP VALUE)
#2= #3026 (TOOL IN SPINDLE)
#3= [2200 + #2] (WEAR COMP IN SPINDLE)
[ #3= #100 ] (SET COMP IN SPINDLE)
M16
M99

What I don't like about this is when we need to apply slight comps (to dial in chamfer or engraving) they would be deleted by this.
 
we touch off by rolling a 1/2" EM under the tool tip, against the top of fixture. Once the EM rolls under the tool tip hit Tool Offset Measure, and adjust length wear by 4.0 (3.5" Fixture Height + 0.5" EM).

OK, I am going to say something here, and I don't give a f@ck whoever gives me grief for it: If yuo have to manually add or deduct anything into your tool length offset field after touching off the tool length, ( Tool Offset Measure ), then your procedure sucks.
For that matter, so does the "misinstructional video" proudly sported on the Haas website for how to touch off tools and work offsets.

To answer your question, look into Setting # 64 : https://www.haascnc.com/service/codes-settings.type=setting.machine=lathe.value=S64.html

No macro, no manual entering, no mental gymnastics.
The jest is this:
1: Your tool length is measured to a fixed point. All tools are measured to the same fixed point.
2: Your work offset Z is the distance between this fixed point and the Z0 of your fixture
3: The two have absolutely NOTHING to do with each other, other than the fixed point in Z.
4: If your workoffsets ( G54, 55, 56 etc ... ) shows 0, then re-read points 1 through 3.
 
I agree with SD you should be setting a work coordinate. Most of my programs have the fixture offsets written in;

G00 G17 G40 G49 G80 G90 G94
G00 G91 G28 Z0.0

(G54 B180)
G90 G10 L2 P1 X0.0 Y7.000 Z1.002 B0.0 <-------
(G55 B000)
G90 G10 L2 P2 X0.0 Y7.000 Z-1.002 B0.0 <-------

M01
N10 T1010 M06

This is for one of the production horizontals but it gives you the idea
 
You are totally right, I needed to take a step back and look at what were actually doing, bad case of tunnel vision!
Thanks guys!
 








 
Back
Top