[Jim Beyer]

First off, I"m a newbie when it comes to programming. But I am learning. I have a program that machines a part. For the side in question, it machines 8 points with a spot drill, uses an end mill to finish the surface area, drills and taps 6 holes and then drills the final 2 dow pin locations. For some reason, these dow pin holes have traveled out of location. Everything else is within tolerance. I have been trying to adjust the X and Y coordinates in the program since all of the tooling on this side of the part uses the same G54.1 P#101 offset. I can get the first dow pin hole to move but the second one won't budge. I determined the coordinates for the dow pin holes by matching the X/Y coordinates with the spot drill tool to the coordinates used by the 5mm drill used for the holes. The program syntax goes as follows:

IF[#1LT1]GOTO9999
(Must start from prog 11 or 12)
(1st x.005 y.002 z-.007)
(2nd x.0025 y-.0076 z .007)
(3rd x-.001 y-.001 z.015)
G90G80G00
M8
M400
N2
(t2 5/8 Spot Drill)
G100 T2 L1 G90 G54.1 P#101
IF[#1NE2]GOTO9002
G51.1 X0.
N9002
G0 X7.0276 Y-2.2492 A0.
G43 Z1. H2 S1500 M3
M8
G99 G81 Z-.190 R.25 F30 P.1
Y.7488 X7.0276
X2.9578 Y1.9635
X-1.371 Y2.1490 Z-.1 F15. (Pin #1 location)
X-1.7667 Y1.9725 Z-.19 F30.
Y-1.9625 X-1.772
X2.9528 Y-1.9625
X2.559 Y-2.146 Z-.1 (Pin #2 location)
G80
G50.1 X0
N1
M432

and then it uses an endmill for the surface, and a drill and tap for the 6 threaded holes and then goes into the 5mm drill for the pin holes:

(T5 5MM Drill)
G100 T5 L6 G90 G54.1 P#101
IF[#1NE2]GOTO9005
G51.1 X0.
N9005
G0 X-1.371 Y[2.1490] A0. (Pin #1 location)
G43 H5 Z1. S5000 M3
M8
G99 G81 Z-.27 R.1 F15. Q.09
X2.559 Y[-2.146] (Pin #2 location)
G80
G50.1 X0
N6


Each pin hole location was off on the X and Y planes. Each hole needed to be moved +.003" in X and Y. The X-1.371/Y2.1490 hole did move when the changed to X-1.368/Y2.1520. The X2.559/Y-2.146 did not move regardless of what the coordinates were changed to. I did change the coordinates in the Spot Drill and 5MM blocks.

I also had another thought about changing what offset the 5MM drill uses since all of the tools on that side use G54.1 P#101. But I can't find where the G54.1 P#101 offsets are listed/located. This is a brother vertical mill 32NB. I access the offsets by hitting the data hard key, the offset soft key which gives me the G54-59 offsets. There is another softkey labeled additional offsets which gives me blocks numbered 1-48. But I don't understand how that is referenced. Meaning if I'm trying to use the first block (#1), is that block called up by G54."1" P#101 or G54.1 P#10"1" or something different entirely. But I think that if I used a different G offset for the 5MM drill, I would also have to use that offset for those relative coordinates used by the spot drill.

Priority for this question would be why the X2.559/Y-2.146 hole won't move or other ways I could adjust it +.003 on X and Y.

Sorry for the drawn out explanation.
Thanks,
Jim

[txcncman]

First, did you change the coordinates for BOTH the spot drill and the 5mm drill?

Second, are you sure the point(s) used for measuring hole locations (such as a milled edge) have not changed and the drilled holes are still in the correct locations?

Apparently this is programmed with variable macro programming (for whatever strange reason). P#101 would be changed by a formula within a program or on the variable page, not the work offset page.

Finally, I think you mean DOWEL pin, not dow pin. I have no clue what a dow pin is. Might want to get a copy of the Machinery's Handbook and brush up on the terminology.

[fordav11]

wow.
I gather you didn't write that program.
What you are doing machining-wise is very simple.
Your program has to be the most convoluted and complicated way of doing it that I've ever seen.

You should simplify it to make it more clear (to you).
Why can't you use the standard G54-G59? (normal workshifts)
Do you need to use G51.1/G50.1? (programmable mirror image)
Do you need to use macro?

The other workshifts G54.1 P1 to P48 should be visible on the offset screen using the PAGE UP / PAGE DOWN buttons but like I said unless you are already using G54 to G59 (6 workshifts all in use) then you don't need to use G54.1 Px anyway.
Also note that P#101 sets the P number not the actual workshift amount. The workshifts would be pre-set on the OFFSET page.

Also G100 looks like a call to a custom macro (for the tool change) so you should back-up your 9000-series macros if you haven't done already.

Calling a workshift is invalid in some circumstances (for example while in mirror mode).
Depending on what is in the macro you may need to put the G54.1 Px on a new line.

What control is this supposed to be for? Fanuc (and which series) or something else?

In any case everything is way way too complicated for a newbie. Try to do it a simpler way using common G-code so you can properly follow what is going on in the program.

[Jim Beyer]

Thanks for the responses guys. Yes, the coordinates for both the spot drill and 5mm drill were changed. The first pin hole moved but the second one did not.

Yes, this program is way too complicated. The fixture for this part was built by an outside source who also wrote the program. Its suppose to run dead on but obviously it doesn't.

The dowel pin holes are measured by a CMM. The CMM program measures all holes for relative position, depth and diameter. Everything is in spec except for the location of the dowel pin holes.

I would have to assume that the variables is what is being used for the offsets. I tried playing around with the extended coordinates assuming that G54.1 P#101 referred to table 1 on that page. That never gave me the correct locations on dry runs. Where would I find the variable page?

The mill is a Brother TC 32B PT Tapping Center. The control panel is only labeled as a Brother CNC Interface.

Please remember, is only one side of the part. The table does rotate on the A axis. They don't want me to change the program, except for correcting the problem with the DOWEL pin locations. Of course.

Thanks,
Jim

[txcncman]

Keep changing the numbers until the location moves?

[christinandavid]

If you want your hole positions to come out correct on a cmm you would need to approach them uni-directionally, drill them 4.7mm, slot drill the top 2mm of the hole and finally ream to finish. That will get them perfect to each other. You would need to use a DTI to check the edges of the part are in position at said A-rotation, for each part if the fixturing is poor.

Also, make sure the part is not being distorted when clamped.

I really do hate being told "don't mess with it unless its wrong"...

DP

[fordav11]

The variable page is usually found via the offset button then MACRO softkey.
But if your control is not Fanuc it could be anywhere. Look in the manual?

I love it when someone says don't mess with it except to fix problems.
Then I fix the problem(s) and when they come back and ask what I did I
tell them only that it's now working fine and don't mess with it

[Jim Beyer]

Yes, txcncman, I completely agree. The changed the second hole location several times. Even made an adjustment of .010" once and it still didn't move.

The "professionals" who built the fixture came in and work on it. They replaced all of the hydraulic cramps, said that should fix it and left.

Holes are still in the wrong location.

I also hate being told not to mess with it. Most of what I know is from messing with something.

The reamer makes sense. I just might have to experiment today.

[christinandavid]

Dont dismiss the other extra steps also. The reason for going to these lengths is to eliminate even the possibility of wandering or backlash contributing to positional error. A reamer will just follow the drill unless you give it a good start. Any error remaining must then be either the cnc out of square, the setup out of square/flat or the cmm planing off a different surface/uncalibrated.

DP

it might be worth doing a test piece using suggested method in a flat and stable test piece. That could eliminate cnc axes being out of square, if you do 4off equispaced holes. If the cmm says test piece is good it must be the fixture/clamping.

[txcncman]

Yes, txcncman, I completely agree. The changed the second hole location several times. Even made an adjustment of .010" once and it still didn't move.

The "professionals" who built the fixture came in and work on it. They replaced all of the hydraulic cramps, said that should fix it and left.

Holes are still in the wrong location.

I also hate being told not to mess with it. Most of what I know is from messing with something.

The reamer makes sense. I just might have to experiment today.

What happens when you change the values 1.000"? How do you know you are changing the correct program or section of the program?

[christinandavid]

There is another softkey labeled additional offsets which gives me blocks numbered 1-48. But I don't understand how that is referenced. Meaning if I'm trying to use the first block (#1), is that block called up by G54."1" P#101 or G54.1 P#10"1" or something different entirely.
Jim

txcncman has just given an easy way of eliminating the program as the source of the error.

Looking again at the pgm I can hopefully help explain why it has been written like this. The programmer seems to have come up with some fiendish way of getting his offsets for each side calculated automatically, so somewhere in the calling program or sub programs there will be a list of variables or a formula where the actual extended offsets to be used will be described. So if #101=6 then g54.1 p6 is being used for this feature, which is offset number 6 in your extended offset table 1-48.

This way of working makes it extremely dangerous for you to change any of the offsets directly until you know where and which offsets are calculated, and which is the original offset or origin every other offset has been struck from. I am interested to know what the comments in brackets at the top of the program refer to. They may describe errors in the fixturing or the machine origin of rotation.

I have to confess I have a system for doing the same kind of thing, but have structured it in a way that actually eases the pressure on my fellow operators (only a single work offset is used) rather than create more confusion by setting multiple offsets.

DP