[MCImes]

Im going to pull my hair out. I program and run a Tsugami swiss lathe with a Fanuc 18i-TB control. Normally it gives me no problems. Till today. Maybe it just knew its Friday...

Im just trying to make a simple .030 radius on the face of my part and my machine refuses to do it. Ive tried it with g42 comp, g41, no cutter comp, changed tools, adjusted the bushing tried making the rad with a different tool...nothing uis working...I need some ideas.

There is a .030 rad on the back side of the part and that is working fine. I thought the stock was possibly being stuck on the bushing at the beginning of the program but ive jogged the stock back and forth before multiple cycles with no problem. Also ive felt for a burr with my fingernail. No burr.

If I program a .100 rad it makes one. however when I go down to around a .050 rad it cuts straight down in X ~.015" then cuts half a 90* radius. so there is a step and half a rad. wtf?

With some of the program versions it makes a chamfer but not to the programmed size. There is clearly a G2/G3 where it makes a G1 chamfer

Things/possible problems Ive eliminated:
-Changed my cutoff and turn tool. Both are sharp and are cutting to size
-made sure there is no burr on the bar
-bar feed torque is high enough that the bar is not slipping back
-main collet is tight enough, but not so tight that it wont release the bar
-Ive tried facing the part with my normal front turn then making the rad with another tool. Same problem. (wtf?!?!?!?!) so Its not my turn tool
-Ive tried it in G42/G3 going from X+ to X-.
-Ive tried it in G41/G2 facing, enabling comp and doing the rad from X- to X+
-Ive tried it with no cutter comp, put like 5 g40's infront of the tool and cheating the numbers .005 bigger.
-Ive changed all my Z- moves at the begining of the program to less than 1mm (bushing to tools distance) so that even if there was a burr it would not get hung up on anything before being pushed off with a g41/g2 rad

Sorry if that is hard to read. Its stream of thought and my thought is Im pissed (or stupid and missing something obvious)
Im out of ideas. Help me!

For reference some of the code that failed is:

M13 S4000
T1515 (FRONT TURN .008 NOSE RAD)
G0 G40 X.53 Z.040
G1 G42 X.500 Z.020
G3 X.440 Z0 R.030 F.0007
G1 X-.02 F.002
W-.005
G0 G40 X1.5 T0

another version that failed:
M13 S4000
T1515 (FRONT TURN .008 NOSE RAD)
G0 G40 X.53 Z0
G1X-.02 F.002
G41 X.439
G2X.499 Z.030 R.030 F.0006
X.503 W.020
G0 G40 X1.5 T0

also tried the same code with no cutter comp. same result...

[danrudolph]

Are you drilling the front of the part?

I've had this problem where I was consistently missing a .015 radius on the front of a part. The bar was somehow consistently slipping .015 in the main spindle collet during drilling, even between setups until I nailed it down.

Crank that collet down to the point where it almost alarms, my guess anyway.

[Sprew]

Circular Interpolation problems boil down to three focal areas.
Where the tool is.
Where its going.
Direction of travel.

The inclusion of cutter comp introduces two more variables. Comp direction & Comp value.

Make sure your stored comp value is correct (.008). Are you trying to radius 90 degrees? Your first example has a Z travel of .02 and the second is .03.

You may need to put in another linear move after turning on the cutter comp. prior to the circular interpolation.

You mentioned a lot of variables. Try to eliminate as many as you can in your problem solving process.

[DCogswell]

Which Tsugami? BS, BE, SS, BO...?
And what tool positions have you tried, have you tried the opposite side of the slide?
Did you verify center height is correct?

Interesting problem you are having, hopefully you'll post your findings and how you solved it.

[MCImes]

Lets see...

-Im confident the collet is tight enough. Ive checked and adjusted it tighter.

-Im not drilling anything.

-Its a BS19-III model which has a single plate with all the tools on it (not like my other machine, the BX with 2 independent slides)

-The machine was running fine as recently as yesterday when I left and it rarely gives me problems.

-Ill check the center height just to be sure but I have no facing nib so It would surprise me.

-As for cutter comp that is the usual lead in move I use to turn it on. X[stock+.030] Z[rad start+.020] in G42

or for g41 i go from X-.020 (facing end) then G41 X[beginning of chamfer]

-Ive never used a straight line move between comp on and beginning of cut so I dont think thats the issue

-The comp value and tool position is correct

-I havent tried the other side of my gang plate but my main front turn tool has always been in T15 with no problems. I figure its got to be something about my setup since ive tried so much different code but ive changed or adjusted everything I can think of...

[DCogswell]

BS19 is old enough...I've seen a radius issue (Fanuc problem and not Tsugami) when using G2/G3 on opposite sides of the slide, even though they are on the "same" plate.

Something to try, instead of going from Z0.00 to Z0.030, try a different portion of the part. Like Z0.100 to Z0.130

This would validate that there is no Fanuc issue or center height or G41/G42 issues...

If that still gives a bad radius, then maybe try to generate on T0404 (I assume you're using T0505 for cut-off)

Also, before you call T1515, do you have a G0T0?

[MCImes]

I like your idea of trying a rad not from z0. Ill turn a little then do a rad and see what happens after lunch in a few mins.

and... yes to g0t0 in the safety line at the top as well a a couple rapid moves to get the cutoff out of the way

and yes to T5 being the cutoff.

If its the control it would be the first time its crapped out on me. This machine is from 2003. The BX12 from 1996 (my other machine) has issues like that all the time and now I just cheat most of my cutter comp moves on it. I hope thats not whats starting here. Its super frustrating to just guess what will make odd geometry work.

At this point ive decided im not stupid and just very angry

[MCImes]

Just did your test and it made a beautiful radius.

I MDI'd in

m13 s3000
t1515
g0 x.51
g1 x.3 f.002
g41 x.35
w.5
g2 x.450 w.050 r.050 f.001
w.2
m5

and it made a very nice rad... so what makes the face of my part different?

It has to be the beginning of the program or the g300 retract? Im using very standard code though... My barfeeder does not push very hard as it a P.O.S. MTA mini swiss but my OAL is correct...

[DCogswell]

Try T0404 just for the confidence that it's not that issue I've seen in the past. When I did see it, it was an late model machine, and it was a Fanuc problem that was rectified by them with a drive swap. I haven't seen it again. But, seeing your issue, I thought maybe this may be the problem.

You said you are generating the .030R on the back side of the part, which tool position is that?

[DCogswell]

Just did your test and it made a beautiful radius.

I MDI'd in

m13 s3000
t1515
g0 x.51
g1 x.3 f.002
g41 x.35
w.5
g2 x.450 w.050 r.050 f.001
w.2
m5

and it made a very nice rad... so what makes the face of my part different?

It has to be the beginning of the program or the g300 retract? Im using very standard code though... My barfeeder does not push very hard as it a P.O.S. MTA mini swiss but my OAL is correct...

Send your code from the beginning of the program to the end of the T1515 process along with your offsets (wear & geometry) for your T1515 & T0505 positions.

[MCImes]

From here------>

O3351
#105=.072(CUTOFF SHIFT)

G65P9002T505D.5S3000M3X-.05F.0015 (bar change/auto cutoff sub prog)
M93351 (SUB PROG)
G0G18G20G40G97G99T0M8
M11
G4U.4
G300X-.05Z3.05T0505
G150Z-.005
M10
G4U.4
G0Z-.05
G0X1.496 (X home)

<------to here is all copy paste code that never changes

M13 S4000
T1515 (FACE/RAD)
G0 X.53 Z.04
G1 G42 X.500 Z.020
G3 X.460 Z0 R.020 F.0008
G1 X-.020 F.0022
W-.005
G0 G40 X1.5 T0


Also I just did an edit just for giggle:

T1515
G0 X.53 Z0
G1 X-.020 F.002
X.250 F.005
W.050 F.002
X-.020
G50 Z0
G41 X.459 F.005
G2 X.499 W.020 R.020 F.0008
X.503 W.020
G0 G40 X1.5 T0

Still the same problem.

I know my tool is nuts on as I did this im mdi:

T1515
M13 s3000
G1 X.400 F.001
W1.
M5

then I measured my cut with the mic with the tool still on the bar and it mic'd .4997.
I still have a G.D. burr and a .003 step at the end of my rad!!!! BAH!

[DCogswell]

Are you sure you are getting .005 of face off, or is it just cutting air? Holding diameter doesn't mean your tool is on center however, with your test MDI cut being successful, I would say this isn't the problem.

4 things:
1) are getting .005 of face off?
2)Change your dwell before M10 to U2.0 (just for now to eliminate a problem with collet closing)
3) Add to your program what you did in MDI to test your G2/G3 in a different "Z" location and see what the radius looks like.
4) and maybe try the same code in T0404

EDIT: write the code and comp the TNR yourself.

T1515
G0G99X.530Z0.00
G1X-.020F.0015
X.424F.003
G2X.5W.038R.038F.0005
G1Z......

[cogsman1]

I am not a Tsugami person but I have seen this type of problem many times
When using "Tool Nose Radius Comp", Make sure you have the correct radius size in your "R" on the offset page and that you have the correct "Vector", usually a "P" , this should be either a 3 or a 4 depending on the machine configuration.
Once you have those correct, you have to understand that when using comp some machines are much more "Picky" than others and need an extra move BEFORE comp is turned on to allow the control to adjust properly. The control looks at the move BEFORE the "G41 or G42" to see where the tool is coming FROM and then looks at the command to see where it is going NEXT, to adjust the tip position correctly.
This is how my machine would cut this radius.
The "Z-.05 and the Z-.02" are to establish the correct direction for comp to work correctly.
SOME machines need this other do not BUT they will ALL accept it so I use it ALL THE TIME!

T1515
G0 X.53 Z0
G1 X-.020 F.002
G0 Z-.05
Z-.02
G1G41X0Z0F.005
X.459
G2 X.499 W.020 R.020 F.0008
G1X.503 W.020
G0 G40 X1.5 T0

[DCogswell]

MCImes, how's it going with your problem?

[tea hole]

My first $.02:
Going from Z.02 to Z0 is not enough distance for the .03" radius you are trying for. Maybe if you had Z.03 in your G3 line you would have better luck.

M13 S4000
T1515 (FRONT TURN .008 NOSE RAD)
G0 G40 X.53 Z.040
G1 G42 X.500 Z.020
G3 X.440 Z0 R.030 F.0007
G1 X-.02 F.002
W-.005
G0 G40 X1.5 T0

My second $.02:
You don't have a G1 on the line after your G2. Most probably not a real deal breaker, but just a thought. As well, i would have my first positioning move to G0 Z-.02 X.53, then G41 to Z0 X-.03 before making your X move to your position before the radius. Again, just a couple of my thoughts/ things i'd try.

another version that failed:
M13 S4000
T1515 (FRONT TURN .008 NOSE RAD)
G0 G40 X.53 Z0
G1X-.02 F.002
G41 X.439
G2X.499 Z.030 R.030 F.0006
X.503 W.020
G0 G40 X1.5 T0