Problem- ECAS32T program optimization

[KentL]

I'd like to discuss program optimization on the Star ECAS32T or any other.
It's new to me and I've run into a problem.

Kent

[PixMan]

What problem have you hit?

I don't have any experience with the ECAS32, but have run optimization on a SR20 RIII. It'll fail if you have any macros in the program, and some of the canned cycles will also kick it out.

What error message are you getting?

[KentL]

Hey good mornin PixMan

Yeah, I've worked through the macro and subroutine issues. So now it runs the optimized program just fine up to where the sub is up on the part to pickoff then it errors out with "Z2 not SYNC CHANNEL 2".
I've tried it with and without the M code for Z1-Z2 sync with same result. This part does not need these synced as it just a straight cutoff.

thanks
kl

[PixMan]

Nuts. I have hit that one myself and can't recall exactly what I did to resolve it. If my memory fails me right (), I think that in typical Fanuc fashion it had nothing to do with the Z1-Z2 synch commands, but the program end codes I was using right after the cutoff.

You might give a call to my friend Chris R over at New England Tool, the Star distributor for my area. Good guy. eight-six-zero six-two-seven seven-eight-three-three

[KentL]

You may be right. We have many Fanuc machines and bogus errors are common. And this being a Siemens control doesn't eliminate that possibility.

I'm going to try a dwell before the collet close and also without the spindle speed syncs. I wonder too if it doesn't like the torque limit code

kl

[PixMan]

Probably that torque limit code!

I was wondering if your machine had a Fanuc or Siemens control. The ECAS 20 I used to program and run had that, I hated it. Poor reliability, worse user interface and the weakest excuse for mating a machine to a control EVER. What was Star thinking with those things?! The reason I go tform a Start technician was "Fanuc controls couldn't handle this many axis' all at once. BS! I ran Citizen M's and Maier ML-E's that had just as many, the Fanuc 16i worked great. Now with the 31i, even better.

[KentL]

I too prefer Fanuc but now that I've got several years with the Siemens I have come to like them. Although I don't care for the way DMG did it on the Twin42.

[KentL]

Success!
It was the M82 spindle speed sync it didn't like. Program now runs 3 sec faster which is only 2 sec off the goal.

Thanks for your input PixMan.
kl

[PixMan]

Originally Posted by KentL Success! It was the M82 spindle speed sync it didn't like. Program now runs 3 sec faster which is only 2 sec off the goal. Thanks for your input PixMan. kl

Cool! Glad you could find it. Now, is there any sign of "skid marks" on the O.D. of the workpiece from spindles that may not be running at exactly the same rpm?

BTW, what material are you cutting, and what inserts (shape, size, tool nose radius and grade of carbide) are you using. I may have a suggestion to get that last 2 seconds (and ten more!) out of the cycle.

[KentL]

Shoot!

I spoke too soon. It runs great right up through the last part. At the first barchange it crashed the cutoff. Apparently there is something in the barchange sub that the optimizer doesn't like. So the trial continues.

FYI;
7/8" 1215 CRS using WNMG 332 wiper @ S4085 F.008 to turn to .748 +/- .0004 with 32 finish.
Also deep 60 deg. carbide spot @ S1600 F.0035. Carbide step drill @ S3000 F.008. 5/16-18 tap @ S1000. Cutoff @ S2000 F.004
This runs @ 43.5 sec normal and 40.2 optimized. Goal is 38.

kl

[PixMan]

Want to run faster? Switch to a Valenite WNMG332 WN3 (wiper) grade VP5615. Run your spindle at max rpm (6000?) but keep the feedrate the same to assure the finish meets the spec. You'll be amazed at the tool life even at that speed.

Very sorry to hear about the crash! Cutoff tools can be pricey. Which cutoff tool are you using? Have you been able to open the cutoff and bar change programs to copy, then break out the macros inside them and bring the code into the main program? I have a suggestion for the cutoff too, one that will run at very nearly the same speed as your turning tool. Just let me know the spec for the toolholder you are (or, were) using and I'll give you my suggested "upgrade".

[KentL]

Thanks. I'll give that a try.

Were using a relatively inexpensive cutoff. Isscar DGN 2202J IC328. Because the cutoff tends to be the most abused and neglected tool in the turret.

kl