Cutter Comp.

[BryGuy]

Mastercam isn't catching all cutter comp. mistakes. We do a lot of profiling with very small radius tools. With a lot on radiuses on the part. The problem is the mastercam post out with cutter comp turned on in the controls and when it goes the the machine we get alarms.

The radius on the tool is to big and can't profile them.

I can give you a quick example thowe ours are more complex and not so easy to spot right off the bat.

 

G42X.0Z.2

G1Z.0G99F.002

X1.0

z-.098

G2X1.004Z-.1R.002 (I HAVE A .008R ON THE TOOL)

G1X1.25

 

Now I have a .008r on the tool with cutter comp turn on in the control and it trying to turn a .002r in that corner. It can be done! I thought M/C V9.0 was set up to find error like this one. And if it's not, I don't understand why they didn't make it to find simple errors like this one. It won't run in the CNC like this. It gives you a cutter comp alarm. Let me know what your thoughts are on this one. Maybe I'm not doing some thing right. I am new to Mastercam.

[email protected]

[JAMMAN]

Personally from experience and my opinion, I have found not all controllers do the math right. I use comp in the computer and avoid G41 and G42 like I would Aids. I used relatively large cutters (120mm) so I had to know exactly where they were going to be at all times and the only way I found was to comp in computer and backplot. Never got an alarm after that.

 

I have experimented with comp in control Vs comp in computer on a jig grinder testing with a Sip cmm. We stopped using controller comp at that company also, it wasn't as accurate.

[PE @ IHS]

Perhaps I am missing something as well, but I am not sure how you expect to turn a .002 internal rad with a .008 rad tool. You would get a comp alarm because the machine knows that this is mathematically impossible. Mastercam might not catch it because when you turn the setting to "comp in control", it simply outputs the drawing dimensions presuming a tool that has no radius (sharp) which COULD cut this part. The CNC is left to make the calculation with G42 turned on, hence the error. Try programming it with TNR turned off and see what the output is.

 

I can't see how it would be possible to create a .002 internal rad (or measure it, for that matter). If your machine is a gang-type lathe (like a Hardinge CHNC), your G02 command actually means CCW arc, creating an external rad. It is still impossible to create it because of your tool size. I am also just learning Mastercam, but I can look at your MC9 file if you wish.

 

Peter Eigler

[JAMMAN]

quote:

---

Mastercam isn't catching all cutter comp. mistakes

---

Mastercam can't second guess the way your controller Interprets comp.

[BryGuy]

I know it's impossable to turn that .002r. That is what I was getting at. I thought that mastercam should let you know you have a misstake. I see what your saying about letting the conputer do the cutter comp. I see two problems with that. One is that when it come to a problem like the .002r, it will just cut it to a shape. And the secound is that we have very very tight tolerances and the radius on the turn would have to be exact. We do profiles with .0003 tolerances + it's stainless steel so it it starts to wear your hights and diam. start to change. It gets very hard to control over a long run..I was just wanting to know if I was missing some thing or not. We need some thing to dubble check us for errors. You would think even if it was in the controls that Mastercam would figure out that you can't put a .002r in a corner with a .008r tool. And Like i said it's just and exsample. I do really try to program it to do that.Because I know you can't. But on some of our profiles it gets hard to make sure the tool radius clears when you only have .008 and .004r insterts to work with.Somtimes it gets tight or boxed it on the profiles and doesn't get caught till it's in the CNC giveing you alarms.

Thanks again

 

[ 05-01-2002, 10:54 PM: Message edited by: BryGuy ]

[JAMMAN]

Dude, when you check comp in control, mastercam assumes you are doing just that- LETTING THE CONTROLLER DO THE COMPING. Mastercam has NO IDEA what you have entered in the tool register on the controller. Somebody please stop me if I'm wrong.

Which post are you using, BTW?

[Fig sign]

BryGuy!

When I started to work as a cnc operator long time ago the first thing I`ve done was to read all Fanuc 6M manuals.

You know what -they had about compensation smthn

like 200 pages!

All this pages where very interesting stuff and they gave me an understanding of the process.

All the machines have limitations in compensation calculation starting with a buffer length or the

mathematical algorithm they use.

So I would recommend you to open manuals and to carefully read about this stuff.

Jamman ,you are pretty right !

When YOU CHECK comp in control , THE MASTERCAM GIVES YOU THE NAKE TRACE only the real dimensions.

It is YOUR responsibility and of your controller.

And when you will not check optimize ,you can have an overcut too ,that is a really bad thing to have.

[MATSSMan]

In Lathe, if you are using control comp, and know there is a possibility of concave radii in the profile that are less than the tool nose radius, use wear compensation, instead of control comp. Then set the radius in the control to the difference between the actual tool nose radius, and the one programmed in Mastercam.

 

When you select control comp in Lathe, the software will program the EXACT profile you chain without regard to the tool parameters.

[P_Scott]

BryGuy,

 

Mastercam will allow for ALL types of compensation, it just can't calculate for the radius of the insert if you have Control comp selected. You could physically put ANY size insert in the machine if you use CONTROL comp. JAMMAN and plasttav are correct. If you use Mastercam to calculate comp, you need to turn it on as Computer or Wear. Wear comp is a combination of Computer AND Control comp. With Computer or Wear comp on, Mcam can calculate the insert radius the user has indicated, is too large to machine that .002" inside radius and will not produce a radius in the toolpath. The only way you could get that radius is if you used an insert with less than .002" radius, regardless of your comp settings in Mcam or at the control.

[BryGuy]

Thanks guys.

 

I was asking all of this because in the post Mplhgt42sp, there in the opitions it said: warren of errors in cutter comp simalation.I turned it to yes.

And in Mastercam V9 you can type in a .008 corner radius and that it's useing the edge of the tool , in the compensation in the tool parameters. (So Mastercam does know what radius is on the tool) Then turn on cutter comp in the controls and it backplots it right and post it right except the .002r thing.

In Mastercam V8 it doesn't backplot or post it right.

So I thought maybe they fixed some cutter comp errors. that is why I was asking and Kinda hopeing they did. I know what your say about the cutter comp in the controls and so mastercam posts it point to point and not worrying about cutter comp, but then agian mastercam does know that tool radius .008 and I told it that. It doesn't take a smart person to see that you can't turn a .002r with .008 tool and should let you know you have an error,or you would think. Or at least I think it should. Thanks agian for all of you help. I'll have to play with the wear control... sounds interesting to me.

 

[ 05-02-2002, 05:38 PM: Message edited by: BryGuy ]

[cncprgrmr]

The best solution for this is to use wear instead of control and set tool tables to zero( +/-.001 ? to comp).This allows the program to do its math at centerline of cutter(better for entry and exit) which in return will ignor what it cannot do at the machine(avoid entering scallops to small).

[Charles Davis]

cncprgmr is exactly right. There is no way this can be construed to be a Mastercam problem.

 

Machine controls are, for the most part, pretty dumb when it comes to calculating cutter comp. No slam against any controller, it's just that mastercam has much more developed and sophisticated algorithms for calculating offset.

 

Mastercam offset calculations, in my experience, are totally flawless.

 

Let mastercam code to the centerline of the cutter, and use cutter comp for wear and deflection only. Most controls work a lot better using this scheme. About 95% of my customers use Wear for precision work.

[Glenn Bouman]

Maybe BryGuy was thinking the Lathe software handles Control Comp the the way the Milling software does which does check and modify the path if the tool rad is greater than the part rad. Maybe Lathe should also have this Optimize switch.

[BryGuy]

that is kinda what I thought In-House

.