PLEASE HELP! :( Lathe Radius Problem

[Tom214moto]

Hi Guys,

Ok, so this problem has been plaguing me so bad that I have decided to hit you guys up on this forum. What is happening is, I set T0202 to make a cut that includes a radius. The problem is, it does not cut the 1/4 arc on the part. Rather, it kind of cuts a 3/4 arc if you follow me. So basically it does not cut the radius at all because it moves away from the part.

Here is the code. (God I feed dumb)

 

%
O0000
(PROGRAM NAME - T)
(DATE=DD-MM-YY - 20-08-20 TIME=HH:MM - 11:12)
(MCX FILE - T)
(NC FILE - C:\MCAMX\LATHE\NC\T.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 2 OFFSET - 2)
(OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG-432)
G0 T0202
G18
G97 S1500 M03
G0 G54 X0. Z.102 M8
G50 S1500
G96 S1500
G99 G1 Z.002 F.0025
X.7483
X1.0619 Z-.0551
G18 G3 X1.104 Z-.0852 R.032
G1 Z-.2375
X1.2454 Z-.1668
G0 Z.1
X0.
G1 Z0.
X.7476
X1.0605 Z-.0569
G3 X1.1 Z-.0852 R.03
G1 Z-.2375
X1.2414 Z-.1668
M9
G28 U0. V0. W0. M05
T0200
M30
%

[nickbe10]

6 minutes ago, Tom214moto said:

The problem is, it does not cut the 1/4 arc on the part. Rather, it kind of cuts a 3/4 arc if you follow me.

Could be a number of things, can you post up an example file?

[Tom214moto]

[JoshC]

24 minutes ago, Tom214moto said:

Radius_Prob.mov

that video doesn't even match your g-code,

 

the g-code file you posted looks like it would produce motion like i show in the image below, so i am not sure what you are trying to show in that video but doesn't look like you are running the same program that you posted on here.

[Tom214moto]

[AHarrison1]

You have not taken the tool nose rad into account. If this code is hand written then you have to add the tool nose rad to the rad you are trying to cut.

I plotted out the x and z co-ord and wrote a finish path with a lathe tool with .03 cnr rad.

You can see that the total rad is doubled, rad to be cut + tool rad.

If I had a smaller tool nose ie .015 then the rad programmed would read r.045.

 

[#Rekd™]

 

1 hour ago, Tom214moto said:

Hi Guys,

Ok, so this problem has been plaguing me so bad that I have decided to hit you guys up on this forum. What is happening is, I set T0202 to make a cut that includes a radius. The problem is, it does not cut the 1/4 arc on the part. Rather, it kind of cuts a 3/4 arc if you follow me. So basically it does not cut the radius at all because it moves away from the part.

Here is the code. (God I feed dumb)

You need to attach the actual Mastercam file not a video.

 

 

[JoshC]

did you try running the machine with the radii output as IJK instead or R?

I would try that, if you open machine definition from the machine tab, then click edit control definition, then on the lathe arc page you can set arcs to output as Delta start to center instead of radii, similar to what was shown in this article here but this article was for a mill, should be about the same steps to get there though even though this shows a mill machine https://cimquest-inc.com/mastercam-2020-control-definition/ 

 

and as mentioned above, a file is worth a lot more to us than a video, can barely even see what is going on in that short video. Let us know if the machine runs properly with Delta start to center arcs instead of radii and if so that would be a easy fix/permanent change.

[crazy^millman]

Seems like it was programmed for Control Comp and Control Comp was not used. 

[AMCNitro]

You need to make sure the tool radius on MC matches the radius on the insert.

[nickbe10]

5 hours ago, Tom214moto said:

The problem is, it does not cut the 1/4 arc on the part.

Could also be your clearance settings. What are the front and back clearance angles, I would be surprised if you could go downhill like that with any thing with less clearance than a 35 degree VNMG, even that might fail.

I take it there is a reason you can't reverse the direction of cut?

[Tom214moto]

Ok, I am back on this stupid radius problem. 

So, The code is correct. It was posted out on our MCam X3

What the machine is doing is basically cutting a FULL HALF RADIUS> Rather then a 1/4 Radius like I would like to see. 

I have gone into the machiine control parameters and still cannot figure out why it is doing this. 

The insert has a .000 Radius on it. I programed it that way to take the guess work out. 

I am working on a different part now. With the last one, I just made it a chamfer. But this is driving me nutty! Need to fix. Any ideas?

[crazy^millman]

1 minute ago, Tom214moto said:

Ok, I am back on this stupid radius problem. 

So, The code is correct. It was posted out on our MCam X3

What the machine is doing is basically cutting a FULL HALF RADIUS> Rather then a 1/4 Radius like I would like to see. 

I have gone into the machiine control parameters and still cannot figure out why it is doing this. 

The insert has a .000 Radius on it. I programed it that way to take the guess work out. 

I am working on a different part now. With the last one, I just made it a chamfer. But this is driving me nutty! Need to fix. Any ideas?

Linearize the code and get ride of the arc to test, but did you reread the comments and do you have answers to them? Sounds like a control issue plain as day to me. You either have comp going on and don't realize it or a programing with comp and don't realize it. A z2g or a sample file at least shows us what your are seeing in Mastercam. Without it we can try a 1000 different things and never solve the problem.

[Tom214moto]

Ok, so below is the code. 

Yes I read all the replies. And no I dont think we have covered the issue. 

I programed it both ways. With Cutter Comp on and off. Only thing that changed was the entire geometry shifted. But it cut the same tool path. 

 

 

%
O0000
(PROGRAM NAME - END CAP TUBE)
(DATE=DD-MM-YY - 10-09-20 TIME=HH:MM - 10:55)
(MCX FILE - C:\DOCUMENTS AND SETTINGS\TOM ERDMANN\DESKTOP\MASTERCAM X3 PROGRAMS\ZRT\END CAP\END CAP GP LARGE\END CAP GP LARGE REV A.MCX)
(NC FILE - C:\MCAMX\LATHE\NC\END CAP TUBE.NC)
(MATERIAL - ALUMINUM INCH - 6061)
G20
(TOOL - 1 OFFSET - 1)
(LATHE TOOL 77  INSERT - THINBIT .06 WIDE FLATE)
G0 T0101
G18
G97 S800 M03
G0 G54 X1.3814 Z-.47 M8
X1.3
G99 G1 X1.12 F.003
G0 X1.3
Z-.4405
G1 X1.2289
X1.2407 Z-.4464
G0 X1.3
Z-.411
G1 X1.2494
X1.2612 Z-.4169
G0 X1.3
Z-.3815
G1 X1.25
X1.2618 Z-.3874
G0 X1.3
Z-.352
G1 X1.25
X1.2618 Z-.3579
G0 X1.3
Z-.3225
G1 X1.25
X1.2618 Z-.3284
G0 X1.3
Z-.293
G1 X1.25
X1.2618 Z-.2989
G0 X1.3
Z-.2635
G1 X1.25
X1.2618 Z-.2694
G0 X1.3
Z-.234
G1 X1.2494
G0 X1.3
Z-.2045
G1 X1.2289
G0 X1.3
Z-.175
G1 X1.12
G0 X1.3
X1.4214
Z-.5457
G1 X1.28 Z-.475
X1.058
G0 X1.4214
Z-.0393
G1 X1.28 Z-.11
X1.058
Z-.18
X1.12
G18 G3 X1.24 Z-.24 R.06********************* Should be 1/4 of a full radius. Cutting 1/2 full radius
G1 Z-.345
G3 X1.12 Z-.405 R.06********************** Same thing. Cutting 1/2 full radius. 
G1 X1.058
Z-.475
X1.064 Z-.472
G0 X1.4214
M9
G28 U0. V0. W0. M05
T0100
M30
%
 

[JParis]

Best solution to see if it's actually in the file is sharing a z2g file..

People can then see the cut and having the control & machine def see if any adjustment might be necessary

[Tom214moto]

Here is the actual file

END CAP GP LARGE REV A.MCX

Whats the z2g file? Never heard of it. 

[JParis]

Click File >> down the menu list Zip2go

Add everything into it and share that

[crazy^millman]

You cannot take a groove operation and try to use it for a turning operations code. That file has nothing, but the groove tool cutting the radius. That tool is defined as a .0935 Wide with a .005R and you trying to take that code and use it on a CNMG tool? Also your part off shank is wiping out the side of the part. You need to define that tool better.

#1 You need to get a hold of your Mastercam dealer and see about getting current . #2 seems like to me you need to get some machine training on how to set it up and use the tools the correct way.

I am giving you a huge benefit of the doubt here since everything screams you may not be a legal user, but if you were not a legal user why wouldn't you have the latest crack version out there and keep using an X3 version. Please don't be offended by that statement we have had several illegal users show up recently and I personally paid for my own seat of Mastercam and do contract programming so I have a big problem with those doing so.

[Tom214moto]

I am a legal user but I let the maintenance payments go. I paid for the software and now its mine. 

Thanks for your help guys. 

[JParis]

1 minute ago, Tom214moto said:

I paid for the software and now its mine. 

Actually it's not but we're getting into the minutiae of the EULA agreement...you paid to lease it for use 

Either way, yes, it's yours to use

[crazy^millman]

17 minutes ago, Tom214moto said:

I am a legal user but I let the maintenance payments go. I paid for the software and now its mine. 

Thanks for your help guys. 

Okay, but were you trying to take the groove code and use it for the CNMG tool?

[JParis]

So I posted that path out of 2020, Operation #8...that's as old I have..

G1 X1.28 Z-.17 F.003
X1.058
Z-.18
X1.12
G3 X1.24 Z-.24 R.06
G1 Z-.345
Z-.405
G3 X1.12 Z-.465 R.06
G1 X1.058
Z-.475
G0 X1.4214

Based on the fact that you have defined the groove tool with a .000 rad and the rad on the corner is .060"

The code is 100% correct

Do you perhaps have a value set in the tool on the tool offset register? That could make what you're seeing happen.

 

Also are you 100% certain that the control wants R's on rads and not IJK values? That can also cause issues.

[AHarrison1]

3 hours ago, Tom214moto said:

Ok, I am back on this stupid radius problem. 

So, The code is correct. It was posted out on our MCam X3

What the machine is doing is basically cutting a FULL HALF RADIUS> Rather then a 1/4 Radius like I would like to see. 

I have gone into the machiine control parameters and still cannot figure out why it is doing this. 

The insert has a .000 Radius on it. I programed it that way to take the guess work out. 

I am working on a different part now. With the last one, I just made it a chamfer. But this is driving me nutty! Need to fix. Any ideas?

What machine are you running this on Tom? i.e. machine age, controller etc

[Tom214moto]

27 minutes ago, JParis said:

So I posted that path out of 2020, Operation #8...that's as old I have..

G1 X1.28 Z-.17 F.003
X1.058
Z-.18
X1.12
G3 X1.24 Z-.24 R.06
G1 Z-.345
Z-.405
G3 X1.12 Z-.465 R.06
G1 X1.058
Z-.475
G0 X1.4214

Based on the fact that you have defined the groove tool with a .000 rad and the rad on the corner is .060"

The code is 100% correct

Do you perhaps have a value set in the tool on the tool offset register? That could make what you're seeing happen.

 

Also are you 100% certain that the control wants R's on rads and not IJK values? That can also cause issues.

So I have ran it both ways. With R and I,J,K values. Still no luck. I aslo checked the control and contacted Fanuc. They told me to check Parameters 4310 and gave me some recomendations. Tried that. Still no luck. 

 

Harrison, this is a Daewoo Lynx 210A with a Fanuc i-Series control. Its a great machine. Dont know why I am struggling so bad

[JParis]

Does this control let you set a tool orientation?

You know, leading edge in a particular quadrant? If so, I wonder if that definition might be off?

I'm grasping here lol