Offsetting offsets?

toolguyfromhell · Jul 6, 2009

I have a VF2 Mill 1995.
We have a 1/2" thick part that locates on a dowel.
The hole is .500" the dowel .499"
The dowel center is G54 X0,Y0
I am outputting a program to machine a shoulder "counterbore" .800"Dia x .120" Deep.
I have ran it with cutter comp, and I have offset the geometry and ran it on tool center.
Each time after running the shoulder the center of the circular pocket is at X.0086, Y-.002
I started by verifying the cam program. The geometry is dead on center.
I then looked into the last few parts ran (totaly different parts/programs), Every hole/groove is off, in the same amount, in the same direction!
I called our Haas service guy, he said it was either G52,or G92. I checked and they are set at 0,0,0
He then said it must be in the program. I looked and the code is telling the machine to run the shoulder/holes/other features, in the correct location.
We have ran several simplified tests, and someting is making this machine run every feature in the wrong place.

Any Ideas?

psychomill · Jul 6, 2009

Check your common shift? (G53)...
Check your G54 work offset?
Program is in fact using G54?

toolguyfromhell · Jul 6, 2009

Not using G53
Code is calling G54

beege · Jul 6, 2009

On an old FANUC, there was an option for a G45-G48 (single increase, double increase, single decrease and double decrease). If you used a single increase in one direction, you had to use it again in the other, or else you'd have a problem with feature location, Knowing zilch about the Haases, I just thought I'd throw it out there. ANybody ever use those codes? Even accidently? Typos?

Want to post the offending program?

toolguyfromhell · Jul 6, 2009

Took a look and G44 length comp-
45,46,48 are not on the Haas Gcode list.?.?

toolguyfromhell · Jul 6, 2009

View attachment ARM.txt

File attached

toolguyfromhell · Jul 6, 2009

I guess i should mention its the first occurance of t05

SeymourDumore · Jul 6, 2009

Toolguy

I'm assuming this is the part of the code:
N76 T05 M06
N77 S616 M03
N78 G00 G17 G20 G40 G80 G90
N79 G53 X-15.Y0.
N80 M00 (REMOVE LH BOLT)
N81 M03
N82 M08
N83 G54
N84 G00 G54 X0. Y0.
N85 G43 H05 Z1.5 M08
N86 G00 Z0.2
N87 G01 Z-0.12
N88 G41 D05 X-0.316
N89 G03 X0.1579 Y-0.2737 I0.316
N90 G03 Y0.2737 I-0.1579 J0.2737
N91 G03 X-0.316 Y0. I-0.1579 J-0.2737
N92 G03 X-0.2296 Y-0.2171 I0.316
N93 G01 G40 X0. Y0.
N94 G00 Z1.5
N95 G43 M09

Well, it looks OK to me, looks OK to NC-Plot and also checks out on ACAD for the points.
Being a .316 programmed radius, I'm making a guess that you're using center line for the program, which would put your tool to be a .168 dia.
Is it possible that the tiny tool is deflecting?
For giggles, try this code in it's place:

T5 M06
G00 G43 H05 D05
G00 X0 Y0 Z.2
S616 M03
M08
G01 Z-.12 F5.
G13 I.316 F2.
G13 I.316 F3.
G01 Z.2 F200.
M09
M05
G00 G49 G53 Z0

It will make 2 passes on the c'bore, so it should be as even and round as possible.

HuFlungDung · Jul 6, 2009

Sure sounds like a bad datum to me. What method is used to dial in the dowel? What is the difference in height between the dial indicator versus the tool, that is how much additional Z travel occurs when the tool comes down to the work? How does the table tram out? Does the machine seem to be sitting level (result of tram test)?

Backlash settings? Bad thrust bearings on a ball screw?

stevo1 · Jul 7, 2009

toolguyfromhell said:
Not using G53
Code is calling G54

I am not 100% on Hass but IIRC G53 is the common and will pretain to any workoffset you are using. So if you have 5." in G53 Z and nothing in G54 Z but call G54 in your program, your workoffset will be 5". IOW G53 is a displacemnt of your home position regardless of what offset (G54-G59) that you call.

Stevo

HuFlungDung · Jul 7, 2009

G53 is the machine coordinate system which serves as the basis for the work offset coordinate systems to work against: you can command moves within that system, but it is not offsettable except by means of G92

psychomill · Jul 7, 2009

You guys are talking the "same thing" but in different apps...

When I mentioned G53, I meant the common or grid shift or all shift, etc, etc... What I forgot is how the Haas display is set up. On the offsets page, Haas refers to the shift by G52. He's already mentioned that it is all zeroes...

I'm with Hu though...

Sure sounds like a bad datum to me. What method is used to dial in the dowel? What is the difference in height between the dial indicator versus the tool, that is how much additional Z travel occurs when the tool comes down to the work? How does the table tram out? Does the machine seem to be sitting level (result of tram test)?

The Datum is awfully suspect and how you're verifying machine position with the part position is curious... Additionaly, are you running a probe? Probing error maybe? If you command your machine to position over the datum pin and you sweep it, are still at 0?

SeymourDumore · Jul 7, 2009

stevo1 said:
I am not 100% on Hass but IIRC G53 is the common and will pretain to any workoffset you are using. So if you have 5." in G53 Z and nothing in G54 Z but call G54 in your program, your workoffset will be 5". IOW G53 is a displacemnt of your home position regardless of what offset (G54-G59) that you call.

Stevo

Stevo.
Tough it does not help Toolguy's problem, but to set the record straight.
On a Haas ( as well as Fanuc AFAIK ) G53 is machine coordinate and is not modal. Invoking it will create movements in the machine coordinate system, INDEPENDENT of any and all active work coordinates, including G92. It has absolutely no effect in any way to any work coordinates.
On a Haas there are 3 and only 3 ways to modify work coords.
They are G52, G92 and G10.
In Toolguys case the program contains no shifts by G10, and he states G52 and G92 are 0.
The posted program also appears to be geometricly correct with rspect to the C'bore.
Now. He did not say that the whole program ( which cuts the entire profile and face ) is off by the stated amount, only that the C'bore is off.
That is why I'd think Hu and Psycho might be incorrect about the pickup location and only a tool deflection is the cause for the deviation.
Of course, backlash or other mechanical issues are also obvious suspects.

psychomill · Jul 7, 2009

Sort of... Terminology is the culprit here....

True, on FANUC and Haas, G53 is "machine". For many FANUC users, the common shift offset (or grid) on the Work Offset page is also referred to as "G53" even though that is not entirely correct. Haas work offset page doesn't display or show a 'common' or "0" offset but displays it a G52.

So what Steve said is correct, just ignore the G53 reference and simply consider the shift. Now, back to your thoughts....

Tool deflection is another possibility... although I'm still curious about how the work offset is set relative to the actual position of the fixture/part. Especially since he stated...

I then looked into the last few parts ran (totaly different parts/programs), Every hole/groove is off, in the same amount, in the same direction!

I took that to mean that there are other features that are out of position and not only the counter bore.

toolguyfromhell · Jul 8, 2009

This is crazy!

Thank you all for the ideas.
I will try to give a concise status. The datum is being set with a rotary coax indicator in the spindle (2 inches longer than the tool), and now being verified with a last word indicator in the spindle (.25" shorter than the tool). The possabilty for the datum (G54) has been ruled out.
We checked the X,Y backlash (twice with diferent indicators) and for an older machine it was suprisingly 0,0!
The table was checked w/ a Sterrett 98 and it is level.
"He did not say that the whole program ( which cuts the entire profile and face ) is off by the stated amount, only that the C'bore is off." To this, I should mention that for the sake of description I tried to simplify the situation. The example program is in fact, machining a waterjet blank. The outside is wjet .03 oversized and two holes are finished (one reamed and the 0,0 hole spline broached). The result is a machined part that is perfect exept for hole locations.

SeymourDumore · Jul 8, 2009

toolguyfromhell said:
The result is a machined part that is perfect exept for hole locations.

I gotta believe it is a tool deflection then!
Is there a reason you cannot go in there with at least a 3/8 EM?

psychomill · Jul 8, 2009

Also... how many splines in the positioning hole? That wouldn't be throwing the part off from the locating pin would it?

toolguyfromhell · Jul 8, 2009

The c-bore is being ran with a .500 Flat. The code is set up for cutter comp.
The program is set up for 4130 steel, we ran that feature on aluminum at the steel F/S and got the same result, that eliminates the tool deflection.
The spline is a 36 tooth and during the testing we have used dummy parts with reamed holes.

toolguyfromhell · Jul 8, 2009

The issue has to be in the controller...some how...
I know there are better machinist out there than I, but this is not a setup issue.
The mill is running the code in the wrong spot.

We have looked at parts ran a week ago and everything is off +X .008-.012 relative to the datum point. The part itself is ok unless it has an existing feature when placed on the mill.

stevo1 · Jul 8, 2009

Is it just the C-bore holes that are off? Could it be the C-bore program? The hole may appear to be a good hole but is it cylindrical or not.

Have you test just picking up the hole with the coaxial set that as 0,0 then move an exact amount like X2. Then drill and ream or center cut endmill using no circular interpolation? Check to see if it is off or even sweep that hole and move and do another. Does it keep moving.

Stevo

Offsetting offsets?

Plastic

Titanium

Plastic

Stainless

Plastic

Plastic

Plastic

Diamond

Diamond

Cast Iron

Diamond

Titanium

Diamond

Titanium

Plastic

Diamond

Titanium

Plastic

Plastic

Cast Iron

Similar threads