Weird machine tool movements

[Michael Reynolds]

This is NOT a problem with mcam, but rather a strange quirk our HMC has. Here's some lines of code:

GO G17 G20 G40 G55 G80 G90 M6 T1

M3 S1000

G43 Z.1 H1 M8

G1 Z-.5 F50.

X-2. F20

Z.1 M9

G0 G91 G28 Z0.

G91 G28 X0. Y0.

M30

What it does, is feed to a z of .1 above the work, turn the coolant off, then RAPID TOWARDS the work before returning to ref zero (g28).

(This is a CELLCON HMC with a Fanuc om control)

In other words, I'm sure this should work, but if I let this code run, I would crash without a doubt.

Any insight?

Thanks in advance!

Mike R.

[This message has been edited by Michael Reynolds (edited 07-19-2001).]

[mopar]

Try this instead...

G90 G80 G49 G40 G17 G55

T1 M6

S1000 M3

G43 H1 Z.1 M8

G1 Z-.5 F50.

X-2. F20.

G0 Z.1 M5

M9

G91 G28 Z0.

G28 Y0.

G90 G55 G0 X0.

M30

good luck

[Reece L Gibson]

Are you using Gage Length or distance from tool change *** to the top of the part

(neg offsets or *** offsets)

Reece

[Scott Bond]

My code looks like mopar's

with T6 M6 it's own line

also we commonly use G43 H1 D1 Z1.

just to be sure some left over comp

from a early tool wont be called up.

But if this is the actual code

I noticed F50. --has the point---

and F20 --did not----

some machines will plunge without the point

hardway

[This message has been edited by Scott Bond (edited 07-19-2001).]

[cadcam]

So mike it sounds like the control does not like the opening statment correct?

is this what your post put out?

Is this a new Machine for you?

i have a few ?'s as you can tell.

trying to get the correct grasp here.

------------------

jay/ aka cadcam

Precision Programming

email: [email protected]

web: www.ppcadcam.com

[lovell110]

GO G17 G20 G40 G55 G80 G90 M6 T1(GO or G0?)

M3 S1000

G43 Z.1 H1 M8(whats your length offset?)

G1 Z-.5 F50.(pretty fast feed)

X-2. F20(no decimal on feed)

Z.1 M9 (where are you going with this??)

G0 G91 G28 Z0.(why no length cancel?)

G91 G28 X0. Y0.(why go from abs. to inc.)

M30 (does this machine cancel on M30)

Mike Im not sure if Im reading this right but Im a little fuzzy on the G20???

[This message has been edited by lovell110 (edited 07-20-2001).]

[This message has been edited by lovell110 (edited 07-20-2001).]

[Reece L Gibson]

Mike, you know most Fanuc's will only allow 3 compatible G codes per line,If you have more than three, is reads the last three and those are the current codes. Single block the program, and then goto the current block page(the one that shows the distance to go) and see what G codes are active.

Try to make sure that when you pick up you TLO that you are in rapid(G0).

When it comes to the F20 with no decimal, the control reverts back to the fixed format, meaning it reads from right to left.So that feedrate is really f.0020,

this goes for coordinate words also. So X1 is really X.0001 Do a test in MDI and find out. Now this applies to Fanuc controls.

 

[Guest]

My question is the code submitted on the forum a direct cut and paste? If so the error with the rapid could be caused by the first line -

GO G17 G20 G40 G55 G80 G90 M6 T1

M3 S1000

G43 Z.1 H1 M8

G1 Z-.5 F50.

X-2. F20

Z.1 M9

G0 G91 G28 Z0.

G91 G28 X0. Y0.

M30

First - change GO (Letter) to G0(number)

Second - Feed rates will need the decimal in the proper place or the machine will feed at .002" per minute from Z-.5" to Z.1 (Fanuc will read as trailing zero without decimal point!)

As far as length cancel, as long as you are calling a length offset for each tool, from the home position, why worry about it? I programmed this way for my entire life and never crashed because of not cancelling the length offset. G20 (Inch Input)

One other thing I had on a Fanuc6MB, the control retained the modal commands Before a canned cycle.

ie

G00X0Y0

G43Z2.H2M8

G01Z.2F10.

G81Z-.5R.2F5.

X0Y3.

G80M9

G91G28Z0

G91G28X0Y0

M99

The machine fed between the holes rather than rapid. Cost us 2hrs of a service call plus milage for the service man. $400 lesson learned. At least they were Canadian Dollars...

Andrew

As much an Enthusiast as James...

 

[Michael Reynolds]

Thanks all, but I'm sure the code is ok. That's even the way it's written in the manual.

Millturn, I'm using G43, entering negative offsets (-10.000), and used both gage length and tool tip numbers. I know they're ok, cuz the machine picks up the numbers and they work. Just when I try to go home do I have a problem.

Jay, nope I wrote this one by hand (the code I typed was just an example)

The zeros are really zeros, the decimal point is really there...I've had nothing but problems with this machine since the beginning....

Thanks all, and I'll try some of your suggestions when I get back to work on Monday!

Mike R.

????????????????????????

[limitless creativity]

This sounds like a software or parameter problem in the control. If a G90 is in the G28 line the machine will rapid down to the program zero before returning to the real ref return. Looks like the G90 is still modal and the G91 is not being seen.

Just my thought.

Mike

[Michael Reynolds]

Yup, big difference between g90 & 91 in this line. But it works now. Don't ask why...Like I've said, I've had NOTHING but problems with this machine being both inconsistant and unrelialbe.

Thanks for all your suggestions!

Mike R.