quick code

H

heartlnd

Aluminum

Joined

Sep 3, 2003

Location

sydney

• Oct 12, 2008

• #1

need help with the following:
i'm trying to use the visual quick code on my haas office mill.no tool changer metric setup.
no matter what i do the z over travel error message appears.i'm trying to engrave sequential numbers on a small job.
thanks for any leads.
[email protected]

 

Donkey Hotey

Titanium

Joined

Dec 22, 2007

• Oct 12, 2008

• #2

Did you set your work offset? Did you touch off your tool length? Do you have any weird values in the wear offsets?

 

H

heartlnd

Aluminum

Joined

Sep 3, 2003

Location

sydney

• Oct 12, 2008

• #3

offset

tool lenght and all offsets were set.that is the strange part.also g20 was set at g21 for metric.

 

W

wrustle

Titanium

Joined

Jun 8, 2006

Location

Massachusetts

• Oct 12, 2008

• #4

How about posting some of your code for us to look at and possibly see where the problem may be?

 

Donkey Hotey

Titanium

Joined

Dec 22, 2007

• Oct 12, 2008

• #5

Is the part thin and sitting down against the table? You might actually be out of Z travel. I recently did a job like that and the cutter was actually about 10mm too short to reach the programmed position.

Does the program run at all or is it a particular move that gives the error? Are you sure the tool you're using is the one that is touched off in the tool table? If you think you have tool #1 but you touched it off as T2, it ain't doing you any good.

 

H

heartlnd

Aluminum

Joined

Sep 3, 2003

Location

sydney

• Oct 12, 2008

• #6

code

here is the sample program
%
O100
(PROGRAM: TESTENGRAVING.NCC)
(DATE: 12/10/2008)
G0 G17 G21 G40 G49 G80 G90
T1 (ENTER A COMMENT HERE.)
G0 G90 G54 X0.0 Y0.0
S2000 M3
G43 H1 D1 Z0.5 M51
G47 P1 X0.0 Y0.0 Z-0.1 R800.0 I0.0 J3.0 F800.0 E200.0 (####)
G0 Z1.0
M05
M30
%

 

g-coder05

Titanium

Joined

Mar 5, 2006

Location

Subic Bay

• Oct 13, 2008

• #7

Wheres your M06? And what are you using the M code option for (M51)? Sounds like your trying to go past your gage line.

 

Donkey Hotey

Titanium

Joined

Dec 22, 2007

• Oct 13, 2008

• #8

It's an Office Mill, without a changer. All he has to do is declare T1. M06 does nothing. The only reason I know this is the Tool Room lathe behaves the same way.

 

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Oct 13, 2008

• #9

I believe your R Value is set at 31" over the work. Try changing R800 to R2.5 for a .1 clearance plane.

 

Donkey Hotey

Titanium

Joined

Dec 22, 2007

• Oct 14, 2008

• #10

Ooohhh...SIM hit on something. He used American units. You're in Sydney. Are your offset pages set to metric?

Also: is this the first time you've used the machine or is this a new problem?

 

H

heartlnd

Aluminum

Joined

Sep 3, 2003

Location

sydney

• Oct 14, 2008

• #11

metric

hi thanks for all your help.well it still does not work.talked to haas in the usa and we're still trying things.i've changed just about everything i can think of.will keep you posted.it's the first time i'm trying this sequential numbering code.

 

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Oct 14, 2008

• #12

Is setting 9 set to Metric?


Can you engrave a literal string G47 PO (1234)?

Did you try G47 P1 (0000)
or
G47 P1 (0001)

See if something happens.


I'll give it a try on mine soon as a machine opens up.

 

H

heartlnd

Aluminum

Joined

Sep 3, 2003

Location

sydney

• Oct 15, 2008

• #13

office mill

well got it going last night.wrote the code by hand not using the quick code from the machine.
%
O00100
T1
G187 E0.03
G43 H01 D01 G01 Z10. F800.
G00 G90 G54 X0. Y0.
S10000 M03
M51
G47 P1 X0. Y-10. I0 J3. R1. Z-0.1 E250 F375 (###)
G01 Z20.
M05
M30
%

and it worked quite good.the only thing to remember to reset the macro variable
#599 back to 1.in order to start the next lot of number from 001 again.
thanks for all the help anyway's
jens

 

M

Macguyver

Plastic

Joined

Jul 15, 2008

Location

Wisconsin

• Oct 17, 2008

• #14

I had the same problem with my toolroom mill. In Visual Quick Code (only) the Z value is NOT negative. Replace your Z value with a positive # and it will run.

This should fix your problem.