What's new
What's new
By:
Advanced search…

Tool Nose Radius Alarm Help

Nerdlinger

Nerdlinger

Stainless
Joined
Aug 10, 2013
Location
Chicago, IL
Hi Everyone!

I recently started using TNR comp when I can on lathes to get familiar with it, even if it isn't necessary. With help from the forum I have had good luck so far but today ran into the dreaded "G41/G42 Interference" alarm (Fanuc Oi). Anyways, I have looked over the code one million times and cannot figure out the problem. I know it is a common mistake for an inside radius to be smaller than the TNR, but the only G03 inside radius on this part is .031 and the TNR is .016. Does anyone see anything wrong with this?? I have the "T" register set to "4", which is proper for this machine (Tsugami B0205)

Thank you!

N20 (FRONT FACING)
M03 S3055 G00 Z0.0 T0202
X0.58
M12
G01 X-0.08 F0.0024
Z-0.04 F0.08
G41 X0.1

N30 (FRONT TURNING)
X0.2 Z0.01 F0.0024 <---stops on this line
Z0.15
X0.2184
G02 X0.2584 Z0.1696 (this has been updated to Z0.170) R0.02
G01 X0.2974 Z1.102
Z1.171
G03 X0.3594 Z1.202 R0.031
G01 X0.455
G02 X0.475 Z1.212 R0.01
G01 Z1.502
X0.492
X0.58 W0.044
G40 G00 X1.4961 W0.0 T0
 
Last edited:
Nerdlinger said:
Hi Everyone!



N20 (FRONT FACING)
M03 S3055 G00 Z0.0 T0202
X0.58
M12
G01 X-0.08 F0.0024
Z-0.04 F0.08
G41 X0.1

N30 (FRONT TURNING)
X0.2 Z0.01 F0.0024 <---stops on this line
Z0.15
X0.2184
G02 X0.2584 Z0.1696 R0.02
G01 X0.2974 Z1.102
Z1.171
G03 X0.3594 Z1.202 R0.031
G01 X0.455
G02 X0.475 Z1.212 R0.01
G01 Z1.502
X0.492
X0.58 W0.044
G40 G00 X1.4961 W0.0 T0
Click to expand...
z is off a tad
 
Its possible that you are trying to comp a sharp corner because the radius on the tip of the tool forms the radius at the corner of the part (programming the radius and trying to comp it). Just out of curiosity have you tried setting R value to something smaller that 0.016, try 0.005 to see if the controller takes it, might be a good indication.
 
Nerdlinger said:
Oops! That is the code from my flash drive...I already tried fixing that to Z0.17 on the control but ran into the same alarm! :wall:
Click to expand...
Hello Matt,
If the Command Block, G02 X0.2584 Z0.1696 R0.02 from your listed program, is supposed to be a blend radius, that is, tangent to the move perpendicular to the machine Centre Line, ending at X0.2184 and to the tapered surface from X0.2584 Z0.1696 to X0.2974 Z1.102, then it doesn't come close. Your tool path in this area creates a small concave feature that is impossible to fit a 0.016 TNR. Following is the Tool Path in the area where your program is failing:

Lathe Comp1.JPG

The following Code may not be correct for your part drawing, but it does result in a Blend Radius at the corner between the perpendicular and tapered line surface. The size and the rate of Taper is the same. However, this code will also raise an alarm in TNR Comp mode due to trying to fit a 0.016 TNR into the the small move of 0.0192 (0.0096 in radius) between X0.2000 and X0.2192. Worse in your example where the end point is at X0.2184

G01 X0.2000 Z0.0100
G01 Z0.1700
G01 X0.2192
G02 X0.2592 Z0.1896 R0.0200
G01 X0.2974 Z1.1020

The following Code will work using TNR Comp and a 0.016 TNR set in the Offset Registry. It will result in a Taper the same as described in your listed program snippet, with effectively, the same Start Point.

G01 X0.2000 Z0.0100
G01 Z0.1545
G03 X0.2264 Z0.1703 I0.0161 K0.0000 (or R0.0161 instead of I0.0161 K0.0000)
G02 X0.2592 Z0.1896 I-0.0036 K0.0197 (or R0.02 instead of I-0.0036 K0.0197)
G01 X0.2974 Z1.1020

With a Fanuc Control, trying to fit a TNR into a Concave Radius that is the same size will result in an Interference alarm being raised when using TNR Comp, hence the reason for a Radius of R0.0161, 0.0001 larger than the TNR, being used to transition into the 0.02 corner radius.

Regards,

Bill
 
Hi Bill!

1. I think I see what you are saying about, "raising an alarm...trying to fit a .016" TNR into the small move of .0192." At first I was like, "who cares how small of an X move it is?" but then I realized that immediately before making the "sharp" turn FROM moving along the Z axis at X0.2 STRAIGHT OUT IN X TO X0.2184 the compensated leading edge of the .016" radius insert would already be at X0.232 (.016 times 2 away from X0.2). So in order to get to the commanded X0.2184 the machine would actually have to move IN in X by 0.0136 (diameter.) thus gouging the part. IS THAT WHAT YOU ARE SAYING?

2. I am not sure of the difference between my program and your first proposed one. Mine will be first:

X0.2 Z0.01 F0.0024 G01 X0.2000 Z0.0100 (NO DIFFERENCE)
Z0.15 G01 Z0.1700 (YOURS IS .02" FURTHER IN Z BUT SO WHAT)
X0.2184 G01 X0.2192 (YOURS IS ONLY .0008" FURTHER OUT IN X)
G02 X0.2584 Z0.1696 R0.02 G02 X0.2592 Z0.1896 R0.0200 (BOTH MOVE OUT .04" IN X AND .0196" IN Z, BUT YOURS STARTS AND ENDS .02 FURTHER IN Z)
G01 X0.2974 Z1.102 G01 X0.2974 Z1.1020 (BOTH END AT THE SAME POINT)

to me it looks like yours is essentially just performing the radius going into the taper .020" further along in Z, but I am sure I am missing something or does that .020" have everything to do with your suggestion?

3. I cannot figure out where the concave feature in your plot comes from. I only see ever increasing X and Z values and the .020" radius G02 move is accompanied with a corresponding .040" increase in X position and .02" increase in Z position:

Z0.15
X0.2184
G02 X0.2584 Z0.170 (Z0.1696) R0.02

Thank you, again, for all your help as usual! If I am understanding your point in my "#1" I will head on back to the factory tonight and give it a shot.
 
BoscoDrummer said:
Its possible that you are trying to comp a sharp corner because the radius on the tip of the tool forms the radius at the corner of the part (programming the radius and trying to comp it). Just out of curiosity have you tried setting R value to something smaller that 0.016, try 0.005 to see if the controller takes it, might be a good indication.
Click to expand...

Earlier I tried reducing it to 0.015 but maybe I'll try going down further just for the sake of trying/learning. Thanks!
 
Nerdlinger said:
Earlier I tried reducing it to 0.015 but maybe I'll try going down further just for the sake of trying/learning. Thanks!
Click to expand...

That will not be enough to prove Bill correct or not.
What you need is something less than half of .0184.
Try the .005 as suggested by Brosco.
 
Nerdlinger said:
3. I cannot figure out where the concave feature in your plot comes from. I only see ever increasing X and Z values and the .020" radius G02 move is accompanied with a corresponding .040" increase in X position and .02" increase in Z position:
Click to expand...

Hello Matt,
The Concave Feature only occurred with your correction from Z0.15 to Z0.17. The Z0.17 is actually incorrect; Z0.15 is right.

Based on a Z0.15 Start of the 0.02 Radius, the following code is correct (your original Code). However, as the Centre of the Tool Nose Radius in X must be at X0.2184 when starting the 0.02 Radius, the actual tip of the Cutting Insert in X must be at X0.1864 (0.2184 - 0.016 x 2) and is the X coordinate the CNC Control would calculate as the compensated X when a TNR of 0.016 is registered in the Offset Registry. X0.1864 is a smaller Diameter than the X0.2000 the tool is starting the Command Block move to X0.2184; accordingly there is just not enough room for a 0.016 TNR without interference.

The following program has the same coordinates as your first listed program and would work without alarm in TNR Comp Mode with a TNR of 0.0092 or smaller registered.

G01 X0.2000 Z0.0100
G01 Z0.1500
G01 X0.2184
G02 X0.2584 Z0.1696 I0.0000 K0.0200
G01 X0.2974 Z1.1020

The following Code will work with any TRN up to 0.016 and uses a Blend Radius between the X0.2000 diameter and the 0.02 corner radius of only 0.0001 larger than the formed radius left by a 0.016 TNR Insert. It will result in a Taper as specified in the program code above, with the 0.02 corner radius being in the same location for both programs.

G01 X0.2000 Z0.0100
G01 Z0.1346
G03 X0.2260 Z0.1504 I0.0161 K0.0000
G02 X0.2584 Z0.1696 I-0.0038 K0.0196
G01 X0.2974 Z1.1020

The program example where the Z0.17 was used as the Start Point and the resulting Back-plot shown in my previous Post (correct for the code using Z0.17), is a good example where the use of the "R" format will stick a Radius in without an alarm being raised, (when geometrically possible) by the control calculating an arc centre based on the erroneous data supplied. In this case the error was obvious, but when the error is not so obvious, the error may not be found until a final inspection is made, or in use. If only a deburr, corner radius, a small error my be tolerable, but if the Radius is important in a profile, then you may have junk parts.

Regards,

Bill
 
Hello Matt,
The following picture may better explain whats going on.

Lathe Comp6.JPG

The Profile shown in Grey is the desired Part Profile with no TNR Comp. The move from 1 to 2 is straight forward, but for the Tool to get to position 4, it must start from position 3. As can be seen from the picture, position 3 would result in Tool and Workpiece interference and its this, via the Look Ahead Blocks used in TNR Comp, that the Control will raise an alarm for.

Regards,

Bill
 
Delw said:
that was my bad, I didnt see you were going into an angle , sorry about that.
Click to expand...

Yeah, I was thinking about that and the Z word should be slightly less than .020 change but then I imagine the X word should be slightly less than .020” also...unless it’s such a slight taper that the difference is negligible. I’ll plot it out...the end point of the G02 could be like X.019999999 from the start point. So I bet the CAM was right in that one.
 
Hello Matt,
At first glance I thought it was the Z0.15 that Delw was alluding to in his earlier Post and that you had corrected that to Z0.17. Sorry for the confusion.

In any regard, what I've explained in my previous two Posts is the reason for the alarm being raised. And yes, the distance from the X Start to the X End point of the R0.02 G02 move is very close to the radius value, at 0.019995628. When programming the part manually, or via a CAM system, the coordinate would be rounded to the closest, Least Programmable Increment of the machine's Control; therefore, the X distance will be 0.02, the same as the Radius value.

Regards,

Bill
 
BINGO! Thank you Bill, Delw, SeymourDumore, and Bosco! I ended up changing the R.02 to R.01, so the X start point for that outside radius became X0.238...a measly .004" further out than the .232" that the tool tip is at prior to the G02 line but "a tenth is the same as mile", right!? In fact, I ran into the same alarm a few more lines down but that was no match for me and my newly-acquired cutter comp knowledge, thanks to you fine people, so I got that one cleaned up in a jiffy. Thank you, again, everyone! :cheers: :cloud9: :bowdown:

IMG_4075.jpg
 
This is a good thread and appears to a great learning opportunity for the OP. Today it's a bit of a luxury to be able come here and have folks of this caliber explain to someone struggling with this "G41/G42 INTERFERENCE" or any comp related alarm or even the fact the alarms are labeled now.

Back in my greenhorn days alone on a off shift in similar situations like to OP and me with no formal training or even a operator's manual. I'd have given my left nut to have a place like this to come ask about situations such as this.

Pardon the interruption, it's just that this post brings back nightmares from long ago. :wall:

Carry on.... :leaving:

Brent
 
Last edited:
Nerdlinger said:
Just an edge break with generous tolerance...and I’m the customer so the best of both worlds haha!
Click to expand...
Hello Matt,
What you've experienced with this workpiece profile is one of the shortcomings of using TNR Comp via the Control on a lathe. Whether the Tool Path is manually, or CAM generated, its created with a Zero TNR implied. Accordingly, the Tool Path will always run with a Zero TNR and failure to proceed being detected only when the actual TNR to be used in the program is introduced.

Most, if not all, CAM Systems would report that, based on the TNR specified, its not going to fit into particular areas, or show an unwanted tool movement, as the picture in my previous Post shows. If you were creating the program manually, calculating the true position of the tool with consideration of the TNR being used, then you would soon see that the TNR won't fit in the area of your program that includes the 0.02 corner Radius.

With a Milling Program, TR Comp is required to dial in and maintain feature size when using the periphery of an End Mill. With a lathe application, size is generally obtained using an Offset to bring the tool closer, or further away from the machine Centre Line. The main advantage of using TNR Comp with a Lathe, is the ability to change to another TNR without having to recalculate the Tool Path and the program being a little more relatable to the part drawing. However, plain diameters will relate directly between program and part drawing irrespective of whether TNR Comp at the Control is used or not. With your original program example, the acceptable TNRs would be limited to 0.009 down; so no big advantage from being able change to another size TNR Insert.

Regards,

Bill
 
You must log in or register to reply here.








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top