Cutter Compensation on Lathe

[Joels]

Since i am a old (44) APT programmer we used to use the center of the radius on the insert tip to create the tool path. When i use the Lathe it defalts to the cutter edge and i always change it to the center of the radius to make sure i get the shape i am looking for. The question is does every do the same as i do and use the cutter radius? and if i create my own tool library will it be saved using the cutter radius when i call that tool from the library?

[chris m]

maybe I'm dense, but could you rephrase that a little? I'm not sure I'm catching your drift..

[Jack Mitchell]

watermaker,

 

Typically we used the center of the insert for mathematically calculating the tangency points, from here we calculated the actual X & Z coords to produce the part.

 

I don't think it advisable to modify the existing tool libraries; others might want to chime in on your inquiry since I don't really use Mastercam lathe very much.

 

I never used APT but I am very familiar with point to point lathe programming without the use of toolcomp.

 

44 ain't all that old IMHO.

 

 

Regards, Jack

[Joels]

maybe i was confusing. not the first time. In APT we always used the center of the radius in the lathe to machine parts. When i use mastercam lathe it defalts to the edges of the insert and i always have to change it to the cutter radius. I was wondering if anybody uses the cutter edge to program? and why? is there a way to make it a default to pick the cutter radius when i select the tool?

[Jack Mitchell]

watermaker,

 

Almost everybody uses the tangency and not the center of the insert.

Realistically, why would anybody want to program the center point since this does nothing useful IE: cutting with recognizable numbers.

 

As I stated previously, the center is only required for mathematically establishing the tangent of the real numbers required for efficient point to point progamming without using cutter radius compensation (G41 & G42).

 

The relivance comes into play when the operator redily recognizes the numbers and can easily make an edit with requiring my engineering or mathematical ability.

 

Please follow Chris Moffatt's response on this thread - only because he cares and he beat the odds a very long time ago. (seriously though, he understands both methods of programming and can help you with this problem).

 

 

Regards, Jack

[gcode]

Alomost everyone programs to the cutter edge

nowdays and it is the Mastercam default.

(The far left radio button on the bottom left of the parameters page.

If you want all your tools comped to the center of the radius, make a new tool library, change the comp to center and save the tool to the library. ( 2nd buttom from the left)

 

Personally, I'd start using cutter edge.

Almost anyone you hire has been trained that way

Every cad/cam system I know of defaults to cutter edge.

Most machine cutter comp is to cutter edge as well.

 

Its easier to train yourself the new ways than to force your employees and cam system to do it the old way.

 

edit:

As Jack siad, one of the best reasons for cutter

edge programing is because it produces man readable code. Cooridnates for straight diameters and vertical faces can be read directly from the gcode. With center radius code you have to calculate every value in your head to compare a program to a blueprint

[Joels]

when you program to the cutter edge i guess you have to use the g41 and g42. i guess this works but i use the center of the radius because it will machine just like i programmed it. the less operator intervention the better. as for reading the program is easy just subtract the cutter radius on Z and subtract the cutter diameter on X. i guess we all do what is best for us. is there a way to set the cutter radius as a default setting?

[Jack Mitchell]

I'm fighting a losing battle here guys.

 

Time for beddy-bye's.

 

Regards, jack

[Joels]

i guess i will have to figure this out on my own.

[randy]

we do mostly lathe work her and we use the cutting edge of insert and every thing works great. mc will automaticly figure the tangent point from cutting edge to give you good code

so you dont have to use radius comp when programming . seems like using center of rad is more work for operator to figure out moves to follow program but what ever way works best for you is how you should go but i would not change your tool lib

[PE @ IHS]

When you comp to the edge of the tool, you do not need to use G41 or G42 (unless you want to). I would advise against using G41 or G42 on a lathe unless absolutely necessary. The software compensates for the difference in TNR on various tools. The point that is programmed is the theoretical intersection point of the 2 axes that you touch off when you measure the tool. The radius of the tool is taken care of by Mastercam, provided you defined the tool accurately. If you use G41 or G42, you have to input the corner rad into the offset screen, as well as the direction of compensation. This is too much hassle in most cases, and you are more likely to get comp errors at the control.

 

Fill in your X and Z geometry offsets and away you go.

[Brendan P]

I also program with tool tip.

As Peter said,mastercam does all the figuring for you.

If I was to start programming with tool nose center,we would have a lotta scrap parts from the guys forgetting to comp the tools!

 

The only problem I see with programming with tool tip is that the posted code is only good for the radius that you programmed your part for.

 

If you ran outta .031 rad. inserts and you had some .015 laying around and had to get the job out the door,you'd have to re-post your code using the smaller radius.

[CNCGUY]

quote:

---

The only problem I see with programming with tool tip is that the posted code is only good for the radius that you programmed your part for.

---

That hasnt been an issue here so far.

What I have a problem with is the operators not reading the setup sheet and using .015 rather than .031, than ask me why the radius or chamfer on the part is to big.

 

First I em then say .

[Harryman]

With many lathes having tool eyes now, programming to center of radius requires additional operator intervention to get the correct offset into the control.

 

In the old days of manual calculations, programming radius center was easier. APT was just old days +1. Back then it also was common for lathes to not have comp.

 

Comp in the computer and touch tool off on edge works good. Code is readable. Tools can be touched off on presetters or workpieces readily, and if the right insert is in the holder, radius comp errors are eliminated.

 

I'd only use control comp if I had a part with close tolerance radius, or angular, features that need to be tweeked in independently from diametrical features.

[Gail Plush / Amcast Automotive]

I use control comp exclusively...For the reasons stated above. I am going to program the next wheel using the edge calculations, and see what happens. I have always wrote by hand with a coordinate print and used different radii to cut the part. In this case it is much easier to use the control to simply "switch" the geometry...

[Philcott]

Watermaker,

 

I, too, must agree with the comments above in regards to using the edge of the tool for programming.

 

That said, I believe I can tell you how to do what you want.

 

Once you have created a finish pass on your part click on toolpath, operations, click on the tool icon and the parameter tab. Now go to the lower left corner and in the compensation window click the circle second from the left. Click ok, and answer yes to the next window's question. Click on the parameter icon, finish parameter tab, make sure compensation type (upper right) is set to computer,click ok, regenerate the tool path and post away.

 

I hope this is what you are looking for.

 

I think if webby was to do a poll on this method of programming we would find almost all the lathe programmers here use the "insert edge" but that is one of the beauties of Mastercam, you can do it almost anyway you choose.

 

Phil

[Joels]

i agree that using the edge is ok but when i do the backplot the corners with edge breaks dont come out right without using a g41 or g42 right?

[Philcott]

Joel,

 

Do you mean graphicaly the corners and breaks don't look right? When regenerating or backplotting, mastercam will show a blue line which represents the theroretical tool tip. If you zoom in and watch closely, the edge of the insert will actually follow the correct path. I am guessing this is what is throwing you off. It sure caused me confusion when I first was using mastercam.

 

Phil

[Joels]

i will upload into the mc9 files folder on the FTP site a program i did using the cutter center instead of the edges. i changed it to the cutter edges if you look at the radiuses they appear to be under cut unless it is changed to s g41 or g42 so i must be doing something wrong? the file is example.mc9

[Philcott]

Joel,

 

I had a look and the file looks good to me. Can you explain what makes you think the rads are undercut. The blue or red line that follows the toolpath is NOT the cutters edge but the theorhetical tip. Read my last post as I believe it will explain for you.

 

Phil

[Brendan P]

quote:

---

That hasnt been an issue here so far.

What I have a problem with is the operators not reading the setup sheet and using .015 rather than .031, than ask me why the radius or chamfer on the part is to big.

---

This is what I'm trying to say,that you need to us the right radius tool for the code that it was created for.

 

Either way,the operator is payed to read the set up sheet and pay attention to what radius insert they choose or how much offset value they comp. their tool.

[Mike Mattera - TFM]

In Mastercam lathe you always want to program to the theoretical tip (the intersection of the X Z cutting edges) and let Mastercam do the nose comp. Most machines have too many rules for comp and Mastercam has none.

 

Mike Mattera

[Mike Mattera - TFM]

Brendan: You have operators who can read???

 

You must be paying top dollar dude!

 

Mike Mattera

[chris m]

Alright, now I know what we're talking about; sometimes I'm a little dense. Brendan, if you quote that last line and add a wiseass comment I'll kick your a$$.

 

I agree with the general consensus that

1) tool tip definition good

2) TNR comp [g41/g42] bad

 

I looked at your file and agree with Phil that the toolpath generated for the large outside radius looks correct. The blue 'undercut' line is the path that the machine will drive but the resulting part will be correct because the nose radius is traveling along the correct profile. If you Step the Backplot to the top of that radius and then zoom in tight on where the tool is, Backstep a couple of times and you'll see that the insert is traveling the correct path.

 

C

[Joels]

ok i think i understand now. thank you all for you patience and help. When i backplot the finish pass on the big radius the line it the theoretical intersection of the cutter edges right? and since mastercam knows the cutter radius it will still drive the cutter on the correct path right? Sorry about the confusion here as i am still learning.