Cutter Comp for turning tools

[Dave.L]

Hello All,

 

For milling, we use wear comp so that the toolpath is programmed to centerline of the tool. I am sure this is the method most use. Using center of the tool only requires us to touch off our tool lengths and leave the diameter offset equal to zero. We adjust our diameters with the wear offset.

 

With that said, I am hoping to do the same with turning tools so we don’t need to enter any offsets in the control other than X, Z and radius as wear only. We currently program our lathes at the machine and we are entering the nose radius for each tool.

 

So, my question is can this be done for turning and are any of you guys doing so?

 

BTW, this is not a MC question, just a question on the tool nose requirements.

[Justin Beebe at Folsom Tool]

Dave,

 

Im not sure about turning but for milling when I climb cut I set the compensation direction to left and set the compensation type to wear if I want to use cutter comp. At the machine I have zero in the geometry column for diameter and make fine adjustments with the wear column. When using this method I look at it like the toolpath is programmed to the edge of the tool not the centerline of the tool. I just want to make sure I understand what you are asking because you say you use wear and are programming to the centerline of the tool.

 

Hope this makes sense.

[Dave.L]

quote:

---

Dave,

 

Im not sure about turning but for milling when I climb cut I set the compensation direction to left and set the compensation type to wear if I want to use cutter comp. At the machine I have zero in the geometry column for diameter and make fine adjustments with the wear column. When using this method I look at it like the toolpath is programmed to the edge of the tool not the centerline of the tool. I just want to make sure I understand what you are asking because you say you use wear and are programming to the centerline of the tool.

 

Hope this makes sense.

---

Justin, you are doing exactly what we do. And, you may not realize it but your toolpaths are the centerline of the tool not the edge of the tool, take a good look you will see.

 

This method is great for a few reasons:

 

1) no need to enter a tool dia in the control.

2) Cutter comp will only be a few thou and most likley you will not get cutter comp errors.

3) tool path is almost exactly what you see since the comp is so small.

[Justin Beebe at Folsom Tool]

Dave,

 

We are talking about the same thing just wording it differently. What I mean is that my tool isn't driving down the center of the geometry I chained. It is offset half the diameter of the cutter so there is no need to put an entry in the geometry column at the machine. So when I say the edge of the tool I mean in relation to the geometry I chained. I agree this is the best method although the great debate of wear vs. control cutter comp comes on the forum quite regularly. Hopefully someone will get you an answer to your real question. I don't mean to get off topic.

 

Have a great Easter

[Dave.L]

Justin, no problem w/ OT at all.

 

This method is just referred to as centerline toolpath.

 

When I first started using MC, we DID NOT use wear - BIG MISTAKE. One day I tried dropping a .25 Emill in a .28 hole using regular cutter comp. Guess what, it does not work since the cutter shift is too great.

 

That example was enough school for me to use wear 100% of the time.

 

PS, Happy Easter too you as well

[kunfuzed]

This exactly what we used to do when I last used lathe in 8.1. Then I think it was selct computer and comp side left or right. It may be different now.

[mcpgmr]

We use computer for lathe. Some guys don't like to see g41 or g42 in the code. I give em what they want. I feel like I work at Baskin Robins. 31 Flavors of programs to choose from. Happy Easter!!!

[Goldorak]

quote:

---

We use computer for lathe. Some guys don't like to see g41 or g42 in the code. I give em what they want. I feel like I work at Baskin Robins. 31 Flavors of programs to choose from. Happy Easter!!!

---

same thing here

 

our lathe guys don't like the wear comp (ask me why , it's too complicated to set 0.000 in cutter comp) they prefer entering the true TNR

 

 

i ending to use wear and set TNR at 0 in mastercam tool defenition

 

that way verify don't show wacky thing like it did in control comp

 

and yes it's an other work around ......

[BBprecise]

To many ways to kill the same bird.

 

On the mills we program to part profile with the X/Y zero's at the same location that print dim's are coming from (comp. type = control, direct. = left, comp = tip.) This way if the operators see an X-2 they can find the feature on the print easily. This works well, so if the oper. has to adjust CC he can tell he's changing the right tool because of the size listed in the tool table.

 

Lathes, we use comp. direction = left, type = computer, and I select the TNR thats on the s/u sheets (seen to many oper's that can't remember the simple things). Our s/u sheets spell everything out. The engineers decide, I prg., they run it. The only real hassle is if we have to change the TNR, I have to redo the toolpath.

[Dave.L]

quote:

---

The only real hassle is if we have to change the TNR, I have to redo the toolpath.

---

Perhaps, but if you need to make parts with tight tolerance radii or angles then I don't think that will work.

 

We plan to use cutter comp but my question is:

 

Anyone programing lathes to centerline of the tool and only using wear offsets for minor adjustments (and not setting tool nose rad)?

[Bryan Johnson]

quote:

---

Perhaps, but if you need to make parts with tight tolerance radii or angles then I don't think that will work.

---

I disagree.

Unlike for Mill, with Lathe, using Cutter Comp (G41/G42) and holding size are two completely different issues.

I would argue that because with (G41/42) you are relying on the machine control to perform complex adjustments to your programmed path, that the ability to produce reliable and accurate parts is sacrificed (not improved).

 

I see only 2 advantages to G41/42 on lathe, and neither apply to offline programming.

1. Ease of manual programming.

2. Ability to change TNR at control without modify of program.

[Dave.L]

quote:

---

2. Ability to change TNR at control without modify of program.

---

Yes, and not just from a .008" rad to a .016", more like an insert that has a .008" spec and it comes in at .007".

 

Say you are profiling a radius and the value a tight tolerance, how else are you going to adjust it without cutter comp