[elaganis]

Anyone have this problem:
When using the conversational programming on our lathe I notice it will only run a finish pass once. And when running a Chamfer (or radius) on a part the roughing part of that program seems to plunge too deep. This "last" pass finish never cleans up.
Is there a way to change that? Maybe it's too much to ask to control the finishing depth but what about the number of passes???

-EJ

[Geof]

Use the G72, G71, G70 routines and you can completely control both roughing and finishing operations.

[::Andy::]

Just got a TL1 last week and i noticed the same issues. Even when i got the guy who runs a Mori over to see if he could figure it out he couldn't. I was using standard G71 code not the conversational. It also depicts it in the graphics.

I'm doing a training day on the machine at the UK Hq of Haas I'll see if i can manage to do it while i'm there and ask them about it.

Andy

[Geof]

Just got a TL1 last week and i noticed the same issues. Even when i got the guy who runs a Mori over to see if he could figure it out he couldn't. I was using standard G71 code not the conversational. It also depicts it in the graphics.

I'm doing a training day on the machine at the UK Hq of Haas I'll see if i can manage to do it while i'm there and ask them about it.

Andy

Can you post a copy of your program? I use G72, G71 and G70 a lot and don't have problems. I would be interested in comparing your code to the way I do it.

[::Andy::]

Can you post a copy of your program? I use G72, G71 and G70 a lot and don't have problems. I would be interested in comparing your code to the way I do it.

OK, will do when i get a chance. ATM its being used as a seconded op machine and hasn't yet been used. I'm technically a miller and run a Haas Mini Mill. This is the first steps i've taken into turning and all i was doing was doing some outer dia in brass with some radius and chamfers. When the cutter on the roughing cuts came to a radius it went into the radius and removed the material needed to complete it. I noticed it on the graphics and showed it to my foreman and he didn't understand either.

I do have another question that i would appreciate being answered without trying to hyjack the thread. When i wanted to put a radius on an outer corner i had to enter a negative r to get it to roll round, other wise it would act as though i was putting an inner radius. Any ideas?

Sorry i'm not very good with all the turning lingo, i'm literally just starting with the whole cnc turning.

Andy

[JWK42]

I am assuming you are starting below the OD of the part and then moving to the face. Then move up to the OD and generate the radius and then turn the OD

GOO X1 Z2.5
G01 Z2 F.01
X1.5 R-.02 F.004
Z0

The -R tells the control that you want to continue in the Z minus direction after rounding the corner. You have to continue at least the amount of R before changing directions again.

G00 X1.5 Z2.5
G01 Z.25 R.03 F.005
X1.75 R-.03
Z0

The positive R tells the control that you want to continue in the X plus direction after rounding the corner. The R move direction is always along the axis not stated in the program line.

I hope the helps

[::Andy::]

I am assuming you are starting below the OD of the part and then moving to the face. Then move up to the OD and generate the radius and then turn the OD

GOO X1 Z2.5
G01 Z2 F.01
X1.5 R-.02 F.004
Z0

The -R tells the control that you want to continue in the Z minus direction after rounding the corner. You have to continue at least the amount of R before changing directions again.

G00 X1.5 Z2.5
G01 Z.25 R.03 F.005
X1.75 R-.03
Z0

The positive R tells the control that you want to continue in the X plus direction after rounding the corner. The R move direction is always along the axis not stated in the program line.

I hope the helps

Thats brilliant! Thank you!

[GAS]

All you have to do is edit the outputted code. Push the MDI key and find the line of code in the program "G71 P10 Q20 U.000 W.000 D.050 F.010" The U & W are the amount of stock that you want to leave on the O/D and the Face. The D represents the depth of cut that you want to take.

[elaganis]

IF i use a G70 P10 Q20 how can I control the number and Depth of the finish passes easily? I've set my G71 U's and W's to .015" each but want 3 finish passes at .005 each?

[Geof]

IF i use a G70 P10 Q20 how can I control the number and Depth of the finish passes easily? I've set my G71 U's and W's to .015" each but want 3 finish passes at .005 each?

Three finish passes is a contradiction in terms; the first two passes are roughing, you can only have one finish pass.

[qualitytool]

follow the g71---------- with a g70 to finish id/od

[::Andy::]

Finally got around to getting the program i was running off the machine.

The G71 code i used was

G71 P90 Q190 U0.5 W0.1 D.75 F.2
N90 G0 X-0.5
G01 ZO. F.2
G01 X9.5 R-1.5
Z-7.5
X13.5 R-1.
Z-12. R1.
X19.5 R-1.
Z-20.
N190 X26.

Theres bound to be mistakes in there but this is just some diameters and radius i programmed to see what i could do.

When veiwing on Graphics the Z-12. R1 part the tool on a roughing cut removes the material from the very front edge of the radius.

Thanks for any help, like i said i'm going to a training course at Haas uk so hopefully I will be a bit better at programming.

Andy

[GAS]

Andy, you are correct. The roughing cycle undercuts the rad at the Z-12. because the control egnors the R in the roughing cycle untill the last pass creating this under cut. I do not know why this is but I will have it looked into. Here is a program that I wrote that acomplishes the same thin with just a few more lines of code.
G00 X26. Z2.
G71 P10 Q20 U.2 W.05 D2. F.26
N10 G00 X-.5
G01 Z0 F.13
G01 X6.5
G03 X9.5 Z-1.5 R1.5
G01 Z-6.5
G02 X11.5 Z-7.5 R1.
G03 X13.5 Z-8.5 R1.
G01 Z-11.
G02 X15.5 Z-12. R1.
G01 X17.5
G03 X19.5 Z-13. R1.
G01 Z-20.
N20 G01 X26.
G00 Z100.
M30
I hope this helps Gary.

[::Andy::]

Cheers Gary, I went to the training centre over here in the UK and got there with plenty of time so I had a chance to ask several question and that.

The Haas engineer/trainer basically said that in a G71 cycle it will ignore a positive R, along with a C as used in Fanuc to create a chamfer. Its a shame but he said it was just the way the software is, although the C isn't used because thats the 4th axis i think with a live tooling machine.

The other issue i was having that is off topic was trying to generate a D hole for rackmount sockets. I was having an issue when trying to use cutter compensation and it would not go back to the point where i want to take the comp off. Turned out i wasn't replacing a G01 after a G03 move, boy did i go red!!!

[CNCADEPT]

Dear Elaganis, reading thru the thread I noticed that you have obtained great input from other colleagues. I am an Applications Engineer at the Haas factory and I would like to invite you to use our department as a resource that is available to you and all other Haas machine, owners, operators, trainees, etc.
It is our goal to provide immediate technical assistance to our customers when it comes to keeping our machines productive and in great running order.
Please feel free to contact me directly for any doubt or problem you might have and I will gladly find a quick solution to your problem.

Best regards,

Milton Ramirez
Applications Engineer
Haas Automation, Inc.
[email protected] <mailto:[email protected]>
www.HaasCNC.com <http://www.HaasCNC.com>
Tel: (805)278-1800 X7127
Fax: (805)278-8561
Toll Free: (800)331-6746

[CNCADEPT]

Dear Elaganis, reading thru the thread I noticed that you have obtained great input from other colleagues. I am an Applications Engineer at the Haas factory and I would like to invite you to use our department as a resource that is available to you and all other Haas machine, owners, operators, trainees, etc.
It is our goal to provide immediate technical assistance to our customers when it comes to keeping our machines productive and in great running order.
Please feel free to contact me directly for any doubt or problem you might have and I will gladly find a quick solution to your problem.

Best regards,

Milton Ramirez
Applications Engineer
Haas Automation, Inc.
[email protected] <mailto:[email protected]>
www.HaasCNC.com <http://www.HaasCNC.com>
Tel: (805)278-1800 X7127
Fax: (805)278-8561
Toll Free: (800)331-6746