Bullnose program error

[JIM ZACK]

I've come across a puzzling problem when I program a contour to be cut with a bullnose end mill. I'm running V9.1 MR105 and running the program on a Haas VF3. The toolpath with the bullnose End mill will not run on the Haas- I get an alarm "Program Error". However, when I repost the exact same program with the only change being that the tool is changed to the same diameter flat end mill, the program runs fine. My initial thoughts are that the problem is with Mastercam and not the Haas but I could be wrong. 'Any ideas?

[Paul McGarr]

2d or 3d contour?

Cutter comp in control on or off?

Details on the program error at the machine?

 

If the code is small enough, post both the working version and failing version here, and we can take a look.

 

Are there any splines in the contour?

 

What are the tool diameters?

 

What is the smallest inside radius in the contour?

 

Paul

[Lee.]

Are you sure you don't have the same error on other tooling?

 

Sounds like a machine issue here.

 

I'd be interested in knowing the following.

 

If you have your filter set to output arcs in all axes combinations, does your machine accept this.

 

Paul, the other points you brought up should not make any difference, just means that the job may not be completely machined is all.

 

Are you calling your tool correctly on the machine?

 

HTH

[Paul McGarr]

quote:

---

Paul, the other points you brought up should not make any difference, just means that the job may not be completely machined is all.

---

Assuming you know everything about what he is doing from the tiny bit of info he gave us, I guess you could be right.

 

I can think of a reason to make each of my questions relevant.

 

Paul

[JIM ZACK]

i guess my initial posting was kinda sparse on details. For some reason I cannot get any toolpath that has a bullnose tool assigned to it to run. Each time the Haas alarms out with "Program Error" with no further details. I first noticed the problem on a simple 2D toolpath using a 1/2" diameter Bullnose with a .06 radius. When I verified the toolpath it looked fine and posted normally. However the Haas choked on it. Cutter comp was in the computer. When I called the bullnose a flat end mill, Mr. Haas liked it and ran the toolpath. The same thing happened when I tried to run a 3D contour toolpath with a bullnose- verify and posts okay but won't run on the machine. I still believe that there is something in my programing and not with the machine.

[jeff]

Jim,there has got to be more to the alarm than just "program error"?!?!

Is there a way to check the diagnostics to see exactly which alram is on?

I'm not familiar with Haas controls,but it seems to me that the machine doesnt like something.

Post both programs and compare the two.

What is so different? Is there a G code in there that your machine doesnt like?

It's probably something silly like that.

Or perhaps a parameter setting.

Does the program with the bullnose cutter run on any other machine???

[Chris Rizzo]

Just a long shot, are you using a side mount changer and do you have the tool # your calling defined in the tool table? If your calling T2 let's say, and there's no T2 assigned, I THINK you might get that vague error.

 

Next guess-

 

quote:

---

I first noticed the problem on a simple 2D toolpath using a 1/2" diameter Bullnose with a .06 radius.

---

Is the toolpath 2d to a depth where the .060 rad is irrelevent (i.e. .250 deep) , or is it cutting like .010 deep, where the tangent point of the rad is computed.? Cutter comp set left/right properly in this regards, too?

 

Have you tried running the program that works just fine with a flat tool, and then change ONLY the tool defination to a bull, and see what happens...none of these should really matter, just trying to look at some sort of other symptoms.

 

I vaguely recall seeing a generic "program error" message when the machine starved on data, or my dnc parameters were wrong. How are you feeding the machine? Should'nt matter what kind of tool your using, but yet another long shot...

keep us posted!

[Paul McGarr]

Wouldn't two small nc files, one that works, and one that doesn't, be all that we would need to figure out the problem? Post a short file with a 3/8 flat, then the same with a 3/8 bull then paste the code here so we can look at it. It has to be in the NC code right?

 

I don't understand how this can be so difficult.

 

Paul

[Leon-ZA]

On a side note... I picked up a problem using DNC on my Haas VF3...

 

I thought it was data starvation, but I eventually found that some of my tool descriptions were longer than others and that the ( ) comments before the toolchange would actually crash my program because the line was simply too long for the Haas control to accept.

 

Funny enough, it never told me anything like that, but if I shorten those tool comment lines, it runs fine.

[htm01]

i've run into the same thing too many char. in desc. of tool

[Chris Rizzo]

Your limited to 30 characters within ( ).