What's new
What's new

G41/G42 comp for G70 cycle ?

D.D.Machine

Stainless
Joined
Dec 10, 2003
Location
poulsbo, wa, usa
Does the G42 go before the cycle and G40 after the cycle of does in go in the cycle?

Yes I was a good boy and searched before asking. but online and in my programming books have it both ways but both say not to do it the other way.

I`m starting to think it might have to do with the control its being used on?
 
I never use TNRC on the lathe, so take this with a grain of salt.

The logical place is the G41/G42 on the block after the P block (the first G1 move), and the G40 in the Q block.

With the assumption that the G71 cycle will not use the TNRC and I will need to adjust the finish allowances accordingly.

Which is why I prefer to program the TNR into the geometry...;)
 
I don`t use it in G71 but this part has a lot of radiuses and angles and I need them correct and thought it was a good time to learn how to use TNRC in the G70 cycle. I have been avoiding it for years ,,, but I try to Avoid anything to do with lathes most of the time.
 
I don`t use it in G71 but this part has a lot of radiuses and angles and I need them correct and thought it was a good time to learn how to use TNRC in the G70 cycle. I have been avoiding it for years ,,, but I try to Avoid anything to do with lathes most of the time.
I was assuming you were using the same P-Q addresses for roughing and finishing ops. So if you use TNRC, the finish allowances in the roughing cycle will not incorporate the TNR. Potential to undercut or leave inconsistent tool pressure on the G70 pass.

It's parts like that that I want to program in the TNR, so the finish pass takes the same DOC's everywhere. Write the geometry once, and use the same P-Q blocks in G71 and G70.

But I use a CAM program to get the tangent points, so it's really easy to take those numbers and copy/paste them into a program.

Wouldn't want to be without CC on the mill, but on the lathe I just don't bother with it.
 
jancollc
you make a vary good point, but how do you get the offset numbers from the cad drawing? with a mill its just a simple offset but its set off the center of the cutter and on a lathe its set of the edge of the cutter not of the center of the rad tip. ?

I`m feeling like I got a ride to work on the short bus today
 
But I use a CAD program to get the tangent points, so it's really easy to take those numbers and copy/paste them into a program.
It's so easy to do that way and gives you total control -- I have never understood the use of canned cycles that don't do as good a job ...

Wouldn't want to be without CC on the mill, but on the lathe I just don't bother with it.
Preachin' to the choir, fella :D
 
how do you get the offset numbers from the cad drawing? with a mill its just a simple offset but its set off the center of the cutter and on a lathe its set of the edge of the cutter not of the center of the rad tip. ?
Write the program from the center of the tool radius. Was called C/L or centerline or cutter center programming at one time.

Then just do a G92 at the beginning to lie to the machine about where it is driving from. For instance, if your home is at X 10.5 then g92 it to 10.5312 for an .0312 radius tool. Since I almost always used a 1/32 radius insert I didn't change during the program but you could if you had to.

When you go around a corner, connect the tangent points with arcs. Then you get a nice no-burr part.

This is what the "finish pass" macro does but by doing it manually you get finer control. Even a simple cad program makes this level of geometry easy.

If you don't care about that, that's fine but I like to optimize a lathe program.
 
You first need to understand what G70 is.
It is not like a typical canned cycle, doing some calculations or causing specific combination of motions.
It is just a copy/paste operation, at the designated place, of the blocks lying between P and Q, with initial and final moves added to it, from/to the start point. The purpose is to avoid the repeated typing of the same blocks.

Therefore, it is better to insert G41/G42 just before calling G70.
You can also have it in the P-block if this block has some clearance with the first point on the profile (which is the case with type-1 G71/G72.In type-2, we can directly go to the first point in the P-block). I, however, do not recommend this method because it give the impression that G71/G72 are using radius compensation, which they usually do not.

A good reference here, explaining these things in detail with examples.
 
It also needs to be noted that G71/G72/G73 not using radius compensation is NOT really a limitation.
Without radius compensation, these cycles only leave some extra material on the workpiece, never overcutting.
The extra material can be accurately machined by G70 with radius compensation.
 
Some controllers will do very bad things if you even try to use TNC within the P-Q coordinates directly. In that situation it's because the feed-retract-feed-retract changes directions for the comp, so "right" compensation is only applicable in one direction, then when the tool retracts out it would need opposite compensation. My old controller throws up an interference alarm most of the time.
 
It also needs to be noted that G71/G72/G73 not using radius compensation is NOT really a limitation.
Without radius compensation, these cycles only leave some extra material on the workpiece, never overcutting.
The extra material can be accurately machined by G70 with radius compensation.

Hello Sinha,
That is the case with a TypeI profile, but not so with a TypeII profile where the X moves are not monotonous in direction.

The following picture shows a profile with a concave feature being machined with a tool set as a Type 3 tool (the Leading Edge in Z and the point on the Insert closest to the machine centre line). In the picture:

1. The Part Profile is shown in White

2. The coordinates of the profile (those coordinates, X and Z, specified in the Profile Definition between the P and Q blocks) are shown in Light Blue.

3. The TNR is shown in Light Green
and
4. The material Left and Over-cut is shown in Magenta.


G71 - TNR - Comp1.JPG

You can see clearly in the attached picture that material is severely Over-cut by the Trailing Edge of the Tool on first element (right most angled element) of the Concave feature.

Cutter Radius Comp on a mill is practically mandatory, as its via this function that the dimensions of features, cut with the periphery of an end mill, are adjusted. Although it can be said that TRC on a lathe is used to adjust the size of some elements of a profile, its mainly Tool Offsets in X and Z that are used to correct the dimensions of a turned component.

There are many versions of Fanuc G71 cycles that are not documented in the Operator Manual supplied with the machine. FST10, 11 and 12 controls handled TRN Comp quite well in a G71 Cycle, but the control before, and many after the aforementioned models, ignore TNR Comp in the G71 Cycle. Accordingly, the profile shown in the above attached picture would be ruined before the G70 cycle is called to finish the profile.

Regards,

Bill
 
This is how I learned back in 1989 from a Yasnac control on a Mori SL35:
G71P101Q102U.02W.003F.012
N101G00X3.
G01G42Z0.F.006 <---Comp goes here,G71 doesn't use comp, and also any F and S codes.
X3.2Z-.1
Z-4.
N102G00G40X5.M09
X12.Z12.
T0202
G96S1000M03
M08
G00X5.Z.1
G70P101Q102 <--Comp IS used in the finish cycle,along with any feed and speed changes
X12.Z12.
M30
 
jancollc
you make a vary good point, but how do you get the offset numbers from the cad drawing? with a mill its just a simple offset but its set off the center of the cutter and on a lathe its set of the edge of the cutter not of the center of the rad tip. ?
I just define a turning tool with the radius of the insert in the CAM tool library. I set the offset in CAM, based on whether it's a OD turning tool or a boring bar, then create the profile with that tool.

When I code it out, it will spit out the tangent points with the THR comped. The tools are set normally- edge of the insert in X and Z.

It's easier to do than to explain how I do it, but I don't have to make any mental gyrations with the geometry- it's just drawn like the drawing.
 
Hello Sinha,
That is the case with a TypeI profile, but not so with a TypeII profile where the X moves are not monotonous in direction.

The following picture shows a profile with a concave feature being machined with a tool set as a Type 3 tool (the Leading Edge in Z and the point on the Insert closest to the machine centre line). In the picture:

1. The Part Profile is shown in White

2. The coordinates of the profile (those coordinates, X and Z, specified in the Profile Definition between the P and Q blocks) are shown in Light Blue.

3. The TNR is shown in Light Green
and
4. The material Left and Over-cut is shown in Magenta.


View attachment 243242

You can see clearly in the attached picture that material is severely Over-cut by the Trailing Edge of the Tool on first element (right most angled element) of the Concave feature.

Cutter Radius Comp on a mill is practically mandatory, as its via this function that the dimensions of features, cut with the periphery of an end mill, are adjusted. Although it can be said that TRC on a lathe is used to adjust the size of some elements of a profile, its mainly Tool Offsets in X and Z that are used to correct the dimensions of a turned component.

There are many versions of Fanuc G71 cycles that are not documented in the Operator Manual supplied with the machine. FST10, 11 and 12 controls handled TRN Comp quite well in a G71 Cycle, but the control before, and many after the aforementioned models, ignore TNR Comp in the G71 Cycle. Accordingly, the profile shown in the above attached picture would be ruined before the G70 cycle is called to finish the profile.

Regards,

Bill

Hi Bill,

You are right. I had type-1 profile in my mind, i.e., monotonic in nature.
For non-monotonic profiles, interference is always a problem, for which working with the offset profile might be necessary. We had discussed this issue in quite detail some time back.
 
This is how I learned back in 1989 from a Yasnac control on a Mori SL35:
G71P101Q102U.02W.003F.012
N101G00X3.
G01G42Z0.F.006 <---Comp goes here,G71 doesn't use comp, and also any F and S codes.
X3.2Z-.1
Z-4.
N102G00G40X5.M09
X12.Z12.
T0202
G96S1000M03
M08
G00X5.Z.1
G70P101Q102 <--Comp IS used in the finish cycle,along with any feed and speed changes
X12.Z12.
M30

Hello Mtndew,
Your example is a Type I G71 cycle (only X specified in the P reference Block). Therefore, as shown in the attached picture in my previous Post, more material than specified by the W.003 address will be left on the taper due to the TNR; no real issue there.

The same strategy employed with a profile having non-monotonous X moves (like the example in my previous Post) and using Type II G71 Cycle, will result in the part being trashed before the G70 has a chance to take a finish pass using TNR Comp. The only way the part profile shown in Post#16 and not be rubbish by the conclusion of the G71 cycle, would be to apply quite a large X finish allowance with the U address.

Using a 0.8TNR, on an angles surface of 225degs (angles surface being cut with the trailing edge of the insert), the finish allowance in X (as a Radius Value) would be 1.131mm to have no finish allowance whatsoever left on the angled surface and 1.131mm on surfaces parallel to the centre line; not a good result when one should be aiming for uniform tool pressure on surfaces when taking a finish cut.

In my view, if a G71 cycle is going to be used (one in which TRN Comp is ignored), its a better, simpler option to incorporate the TNR comp in the profile coordinates.

Regards,

Bill
 
Hello Mtndew,
Your example is a Type I G71 cycle (only X specified in the P reference Block). Therefore, as shown in the attached picture in my previous Post, more material than specified by the W.003 address will be left on the taper due to the TNR; no real issue there.

The same strategy employed with a profile having non-monotonous X moves (like the example in my previous Post) and using Type II G71 Cycle, will result in the part being trashed before the G70 has a chance to take a finish pass using TNR Comp. The only way the part profile shown in Post#16 and not be rubbish by the conclusion of the G71 cycle, would be to apply quite a large X finish allowance with the U address.

Using a 0.8TNR, on an angles surface of 225degs (angles surface being cut with the trailing edge of the insert), the finish allowance in X (as a Radius Value) would be 1.131mm to have no finish allowance whatsoever left on the angled surface and 1.131mm on surfaces parallel to the centre line; not a good result when one should be aiming for uniform tool pressure on surfaces when taking a finish cut.

In my view, if a G71 cycle is going to be used (one in which TRN Comp is ignored), its a better, simpler option to incorporate the TNR comp in the profile coordinates.

Regards,

Bill

Correct, it's not perfect, but it is mainly for contours that don't go lower in X, you have to keep going up in X.
On that particular control, if you wanted to do a contour like your picture you would have to insert an R1 on the G71 line.
Now, on newer controls it's different. But I haven't programmed cnc lathes since the late 90's so the conversation side is a LOT better, especially on Okumas.
 








 
Back
Top