Mastercam bug or post issue?

[G Caputo]

Hi all,

I had a little issue at work today and was wondering if anyone else has run into this. I programmed a a simple 1-3/4" diameter counterbore using a 1-1/2" XOMX style cutter that was 3-1/2" deep. I used cutter compensation in the control using a contour toolpath with the ramping function turned on. This was programmed to go on a machine with a Heidenhain Tnc 430 control. When it got to the point where it was to make final pass at depth, the cutter comp lost it's mind and it tried to take a cut at where it was comping wrong. At 48 IPM @ 3.50" deep, lets' just say stuff moved a bunch and other stuff broke a bunch.

 

Well it looked great in verify, looked great in backplot, but it didn't look good in real time. I test ran it at the control after the fact and it came up with a "tool radius too large" error. That is totally understandable and I could see it in the program after the fact. The control in full sequence didn't put up a flag and stop, it tried to run and had catastrophic results. I tried the exact program on a Tnc 426 & Tnc 415 and the machines stopped like they were supposed to . Why the Tnc 430 didn't, I have no clue

 

I programmed it to go .09375" per pass until it was 3-1/2" deep which was 37-1/3 revolutions. If I program it to go at .125" depth per revolution it comes out to 28 passes. I try running that on the control and it is fine. Basically an exact number of revolutions works fine, but revolutions that don't equal an equal 360 degrees I have a crash.

 

What is causing this, a bug with mastercam? A post issue? Anyone have any ideas?

 

Thanks

[Henk]

Hi Greg,

 

We have only 426 here, and an older 407.

IMO its no mastercam bug because the program runs ok on an 426.

Normaly 426 pgm's also run on a 430.

You have to find why the 430 go wrong.

Maybe it's a parameter in the control.

[mayday]

Greg, we somtimes have the same problem on the 430. we have resorted to doing deep helical type cutting using the function at the machine. it may have somthing to do with the number of revs in the cycle. I know hiedi dont like more than 15 revs(i think) per cycle. when it does error its alwasys at the comp off move. you may want to try the z retract before G40

[Henk]

quote:

---

we have resorted to doing deep helical type cutting using the function at the machine.

---

I added that function "208 Helical mill" to my dill operations and use it that way.

[G Caputo]

Mayday,

it's all hard coded programming, no cycles or labels. Here's a snipet of the program.

 

209 CC X+3.4913 Y+3.4913

210 CP IPA+180 Z-3.375 DR+ RL

211 CC X+3.4913 Y+3.4913

212 CP IPA+180 Z-3.4219 DR+ RL

213 CC X+3.4913 Y+3.4913

214 CP IPA+180 Z-3.4688 DR+ RL

215 CC X+3.4913 Y+3.4913

216 CP IPA+119.999 Z-3.5 DR+ RL

217 L X+3.0538 Y+4.2491 Z-3.5 RL

218 CC X+3.4913 Y+3.4913

219 C X+4.3663 Y+3.4913 DR+ RL

220 CC X+3.4913 Y+3.4913

221 C X+3.0538 Y+4.2491 DR+ RL

222 L X+3.4913 Y+3.4913 R0

223 L Z+5 R0 F MAX

 

The 15 times max revolutions or 5400 degrees doesn't come into play at this point. I also do not see anyway to make the program retract before the last pass. This was a contour with the ramp functioned turned on.

 

Henk,

quote:

---

IMO its no mastercam bug because the program runs ok on an 426

---

The program is definitely wrong. The 426 and 415 catch the problem and don't run where as the 430 flags an error in test run, but went ahead and tried to run in full sequence. I will look into the parameters of the control and see if I can't find something.

 

 

I'm still trying to come up with a good reason for this, to me there should be no reason why this did what it did. If I make it even 360 degree revolutions it works correct, if I don't, the tool decides to flop out of the spindle. I'll keep looking into it and see if I can't come up with something better, but as of right now the machine will not run, because there is no way to hod a tool and the control will not allow it to run

 

Thanks

[Henk]

Greg,

 

I looked throug the program lines.

Look at line 217, why is there an linear move?

[mayday]

Greg, can you email the geometry of the contour section. I'll post it with my post to see if it outputs the same.

[G Caputo]

Wes,

I can't find your email, so I couldn't send an attachment. I put it on the FTP under MC9 files as "B - 3802 - FINISH COUNTERBORED FACE". It's operation #3. If you need me to, send me an email and I will attach and send to you if that is easier.

 

Henk,

There is the crash, the program is wrong. I don't know why it put that in there. Like I said, if I do exact rotations of 360 degrees, it doesn't do that.

 

Thanks both of you for the help!

[Allan Brown]

I posted with my current Heidenhain post and had these results:

 

CC X+3.4913 Y+3.4913

CP IPA+180 Z-3.375 DR+ RL

CC X+3.4913 Y+3.4913

CP IPA+180 Z-3.4219 DR+ RL

CC X+3.4913 Y+3.4913

CP IPA+180 Z-3.4688 DR+ RL

CC X+3.4913 Y+3.4913

CP IPA+120 Z-3.5 DR+ RL

CC X+3.4913 Y+3.4913

C X+4.3663 Y+3.4913 DR+ RL

CC X+3.4913 Y+3.4913

C X+3.0538 Y+4.2491 DR+ RL

L X+3.4913 Y+3.4913 R0

L Z+5 F MAX

 

See if your post has a pheloutz postblock.

 

Add a # in front (or delete) this line if the linear move is the cause of the problem:

 

code:

---

if nextz = z, pn, *sg01, pfxout, pfyout, pfzout, pccdia, feed, strcantext, scoolant, peob, e   # Repeat position

---

Older TNC controls apparently lost position on the helical CP IPA moves (?) and needed the position restated. It's commented out by default.

 

[ 03-22-2005, 11:26 AM: Message edited by: Dave Thomson ]

[Allan Brown]

If that line isn't there, or is already commented out, then search for mtol in your post.

 

If it's not there, add this line up around where vtol is initialized:

 

code:

---

mtol        : .000001 #Avoid internal rounding assuming 6 dec NCI

---

CNC Software says to use 5 dec for inch, 4 for metric:

 

mtol : .00001 #inch

 

Then try your same program and see if the line is output or not.

[mayday]

same Greg, this code should work fine in the 430

 

87 CP IPA+360 RL Z-3.375 DR+

88 CC X+3.4913 Y+3.4913

89 CP IPA+360 RL Z-3.4688 DR+

90 CC X+3.4913 Y+3.4913

91 CP IPA+119.999 RL Z-3.5 DR+

92 CC X+3.4913 Y+3.4913

93 C X+4.3663 Y+3.4913 DR+ RL

94 CC X+3.4913 Y+3.4913

95 C X+3.0538 Y+4.2491 DR+ RL

96 L X+3.4913 Y+3.4913 R0

97 L Z+5 F MAX

[mayday]

this is what you get if you enable "retract before last move" on the exit side of leadin/leadout parm.

notice the z move with comp active then linear move with comp shutting off, z retracted

 

 

CC X+3.4913 Y+3.4913

93 C X+4.3663 Y+3.4913 DR+ RL

94 CC X+3.4913 Y+3.4913

95 C X+3.0538 Y+4.2491 DR+ RL

96 L Z+5 F MAX RL

97 L X+3.4913 Y+3.4913 R0

98 L X-3.4913 F MAX

 

 

ps. have you looked at an allied spade to blast those holes before you contour the bottom?

[G Caputo]

Dave,

 

quote:

---

Add a # in front (or delete) this line if the linear move is the cause of the problem:

---

That was it!!! Only one of our posts had that not blocked out and low and behold, that's the machine it was posted for. Thanks a ton for helping me resolve the problem!!!

 

Mayday,

quote:

---

this is what you get if you enable "retract before last move" on the exit side of leadin/leadout parm.

notice the z move with comp active then linear move with comp shutting off, z retracted

---

Thanks for teaching me! I didn't know.

 

quote:

---

ps. have you looked at an allied spade to blast those holes before you contour the bottom?

---

We are lucky if we make one of these a year, so it wouldn't be feasible to me for this part, but I will definitely look into that tool for other things we do. Thanks!

 

Dave, Mayday & Henk,

Thanks to all of you for taking the time out of your day to look into this for me. A big thanks you to all

[G Caputo]

Just a quick update on this issue. Once we got the spindle all fixed and I was physically able to run the program on that machine again, it seems as though the 430 errored out on that line, but only after it ran that line. The 415's and 426's stopped at that line without running. The tool looked as though it was compensating from the id of the hole to the od of the hole. All in all, my post had a problem and the 430 controller also had a problem so error 1 + error 2 resulted in some broken sh$t. Again thanks all for the help and we will see what the fine folks at heidenhain have to say.