What's new
What's new

help with G71 roughing cycle

squinn2185

Plastic
Joined
Feb 8, 2020
Hello,
I was wondering if anyone out there had any advice on how to troubleshoot my roughing cycle. This is a sleeve for a roller assembly that has a deep bore that is 4.1339" long and tapers from 1.83" to 2.283". I tried to dry run it and got an error message of PS0322-finisihing shape which over starting point. I was also getting the error message PS0325-unavailable command in shape program, so I moved my TNR comp to my first rapid movement before I start my cycle which seemed to stop that alarm from happening. Here is my program:

(TOOL 9-DMNG 433-LONG BORE)
T0909
G18 G20 G40 G55 G99
G50 S2500
G96 S1200 M3
G00 G41 X1.9158 Z.100/M8
G71 U.07 R.05
G71 P3 Q4 U.06 W.005 F.012
N3 G00 X1.9158 Z.100
G01 X1.8317 Z-.0722
Z-1.6
X2.2835 Z-.422
Z-4.0709
G03 X2.1575 Z-4.1339 R.063
G01 X1.955
X1.875 Z-4.1739
X1.855 Z-4.2350
N4 G40 X1.83
G70 P3 Q4 F.006
G00 G80 X1.75 Z.100 M9
G28 U0.0 W0.0
M1

any help would be appreciated, not quite sure where to start with this one.
 
You can't make that shape with a G71 cycle. I'm assuming this is on a Fanuc control. G71 cycles don't like to make "reliefs". If the bore diameters in your cycle were continuously getting smaller, it would be fine. The same goes for external turning. If the diameters were only getting bigger, it would work fine, but if they dipped back down to make a groove or relief or whatever, you would get an alarm. It just can't calculate the rough passes without overcutting somewhere. Your best bet is to just program it all out or use the G71 without making the relief. Then program out the roughing of the relief. Then program the finishing without using G70. I hope this helps.
 
This got me thinking that I had read that there was a way to do the profile you wanted with G71.

Check out this article and the one on the next page.

G71 Rough Turning Cycle

Apparently there is a Type 2 G71 cycle that some controllers support that allows you to make the "reliefs" or "pockets". I don't know how to tell if you have that on your controller.

I should also point out that I think your second G71 line should have a negative U value. Otherwise, you will over-cut.
 
G01 X1.8317 Z-.0722
Z-1.6
X2.2835 Z-.422

Z-4.0709
G03 X2.1575 Z-4.1339 R.063
G01 X1.955
X1.875 Z-4.1739
X1.855 Z-4.2350
N4 G40 X1.83

The two lines in red are your problem. You can't go to Z-1.6 and then come back to Z-.422.
 
Hello,
I was wondering if anyone out there had any advice on how to troubleshoot my roughing cycle. This is a sleeve for a roller assembly that has a deep bore that is 4.1339" long and tapers from 1.83" to 2.283". I tried to dry run it and got an error message of PS0322-finisihing shape which over starting point. I was also getting the error message PS0325-unavailable command in shape program, so I moved my TNR comp to my first rapid movement before I start my cycle which seemed to stop that alarm from happening. Here is my program:

(TOOL 9-DMNG 433-LONG BORE)
T0909
G18 G20 G40 G55 G99
G50 S2500
G96 S1200 M3
G00 G41 X1.9158 Z.100/M8
G71 U.07 R.05
G71 P3 Q4 U.06 W.005 F.012
N3 G00 X1.9158 Z.100
G01 X1.8317 Z-.0722
Z-1.6
X2.2835 Z-.422
Z-4.0709
G03 X2.1575 Z-4.1339 R.063
G01 X1.955
X1.875 Z-4.1739
X1.855 Z-4.2350
N4 G40 X1.83
G70 P3 Q4 F.006
G00 G80 X1.75 Z.100 M9
G28 U0.0 W0.0
M1

any help would be appreciated, not quite sure where to start with this one.

I didn't realize you could use optional block delete this way.

Brent
 
(TOOL 9-DMNG 433-LONG BORE)
T0909
G18 G20 G40 G55 G99
G50 S2500
G96 S1200 M3
G00 G41 X1.9158 Z.100/M8
G71 U.07 R.05
G71 P3 Q4 U.06 W.005 F.012
N3 G00 X1.9158 Z.100
G01 X1.8317 Z-.0722
Z-1.6
X2.2835 Z-.422
Z-4.0709
G03 X2.1575 Z-4.1339 R.063
G01 X1.955
X1.875 Z-4.1739
X1.855 Z-4.2350
N4 G40 X1.83
G70 P3 Q4 F.006
G00 G80 X1.75 Z.100 M9
G28 U0.0 W0.0
M1
Hello squinn2185,

There are two types of G71 Roughing Cycles, Type 1 and Type 2. Type 1 only allows for monotonous increase or decrease in X, while Type 2 allows for non-monotonous change in the X Coordinates in the part profile description. Type 1 is utilized by only specifying an X coordinate in the "P" reference block of the part profile description and Type 2 with the inclusion of and X and Z coordinate in the "P" reference block.

In your program, you have satisfied the requirement to be able to cut a Concave Feature (non-monotonous X Coordinates) by N3 G00 X1.9158 Z.100 in the "P" reference block; accordingly, the issue is not related to the pocket feature. However, as Fancuku suggests, a retrograde movement in Z is not allowed. I suspect that is a typo in any regards, as being able to cut such a shape would be highly dependent on the shape of the tool and would require a trailing edge angle of the insert of less than 10.8558dges to the horizontal for the profile described.

Apart from the retrograde Z Movement, the start position of the tool in X before the specification of the G71 Cycle, should be slightly less than smallest diameter specified in the Part Profile Description; in your case, X1.855. As you're stepping off the profile to X1.83, that would be the value to use as your start point before the G71 Cycle.

If the control is a Fanuc control, TNR Comp will be ignored completely in the G71 Cycle. Even if it were to work in the G71 Cycle, you have cancelled it before executing the G70 Block and therefore, the part profile shape will be finished without TNR Comp and the part made into scrap. However, that wouldn't be a worry, as the part would be scrap anyway by the time G70 is executed, due to TNR Comp being ignored in the G71 Cycle.

Regards,

Bill
 
Last edited:
Apparently there is a Type 2 G71 cycle that some controllers support that allows you to make the "reliefs" or "pockets". I don't know how to tell if you have that on your controller.
He has activated Type 2 by putting an X and Z value in the N3 line but like you said, the machine he is using may not be capable of type 2 depending how old it is.
 
He has activated Type 2 by putting an X and Z value in the N3 line but like you said, the machine he is using may not be capable of type 2 depending how old it is.

The issue has Zero to do with Type 1 or Type 2, as p/s 064 would be raised if G71 Type 2 was not available, or if the OP hadn't invoked Type 2 by including both X and Z coordinates in the "P" reference block.

Age of the control also has nothing to do with the availability of G71 Type 2, unless the control pre-dated the FS6 control. The OP's control uses the two block G71 format; accordingly, if its a Fanuc control, it will be at least a circa 80's FS0T control. G71 Type 2 is an option, one that most MTBs include and therefore its broadly considered as standard, therefore, its possible that Type 2 is not included with a control, but this is not the OP's case.

Regards,

Bill
 
Then wouldn't the last move be down to starting diameter?
On bores, I have the last move down to starting dia.
That's correct, but the OP has his Start Dia. at a coordinate (X1.9158) larger than the smallest diameter in the Profile Description (X1.855). That's the reason for the P/S0322 alarm that's being raised.

Regards,

Bill
 
Thank you for your help. Unfortunately I’m still getting both the starting point error message and now the unavailable command in shape program error message is back, I might be at a point where I have to rewrite this program longhand. I can take the TNR comp out of the cycle and then I just get the starting point error.
 
Thank you for your help. Unfortunately I’m still getting both the starting point error message and now the unavailable command in shape program error message is back, I might be at a point where I have to rewrite this program longhand. I can take the TNR comp out of the cycle and then I just get the starting point error.

Have you changed the X starting point (the X coordinate before the G71 Cycle is executed) to less than the small diameter of the part shape? Think about it logically. If you're cutting a profile that has a small diameter of 1.855, you must have drilled a hole, or started with hollow bar with a diameter less than 1.855. When boring a hole that has a diameter less than 1.855", what diameter would you park the tool at? Certainly not 1.9158".

You have two problems that's stopping the cycle from running; your start point is larger than the smallest diameter in the part profile definition and you have a retrograde Z move. Fix those and the G71 Cycle will work. Then all you have to contend with is the TNR Comp you're trying to use in the Cycle. Rewrite the Profile Definition including the compensation for the Tool Radius included in the coordinates. This will then produce the profile accurately, but only if you change the Finish Allowance in the second G71 Block from the following:

G71 P3 Q4 U.06 W.005 F.012

to

G71 P3 Q4 U-0.06 W.005 F.012

The Finish Allowance has to be expressed in size and direction. What you have now will cut the part oversize and you still end up with scrap.


Regards,

Bill
 
I have the starting point at 1.9158 so that I can rough out a 30 degree chamfer at the opening of the bore. I'M drilling the hole with 1.75" drill, then rough boring the chamfer and the smaller bore and finishing the large bore with a fillet and a chamfer on the back side. I'm then finishing the smaller bore with another tool since the 1.8917" bore has to have a finish of 32ra. The larger 2.2835" bore has an F finish so I'm not to concerned with that one. thanks for the advice i will try the corrections you suggested.
 
I fixed the starting point and put TNR comp back into the profile coordinates and I still get the unavailable command in shape program error. I’m not getting the starting point anymore, now just the unavailable command error.
 
Are you still programming a move to Z-.422 after the Z-1.6 line?
AS mentioned above this will give an error. Is it supposed to be Z-2.022?

Z-1.6
X2.2835 Z-.422
 
G71 cycles don't like to make "reliefs".

The very first cnc lathe I learned on was a new 1989 Mori SL35 with a Yasnac control on it.
We had the guy come in for some troubleshooting from Yamazen-Chicago and his name was Saito. Supposedly he wrote the software for that control.

Anyway long story short he showed us that if we put an R1 in the G71 line, it would do a relief cut.
Now will this work on Fanuc? I think I tried but it didn't work, I can't remember.
 








 
Back
Top