Problem posting code

[CNCMike]

Hi Guys,

When I post code in MCX2 using the generic mill I get G54 X, Y, A rather than X, Y, Z. Our Fanuc control does not recognize this and gives me a P/S alarm 009 "Unusable character was input in significant area". Any ideas?

 

Thanks for help as usual!

 

Mike

[john316]

.

 

Check your WCS compared to your T&C planes. You might have a rotation set up by accident.

 

.

[CNCMike]

Thanks for the suggestion. I just checked and the T&C planes are the same as the WCS. This is the first time we have posted code, so it could be any number of things?

 

Mike

[JerryBenoit]

What do you use for your work coordinate system

 

G50 or G92?

[cadcam]

What are you posting a contour. is there a value with the A output or is this just G54 X0. Y0. A0.

 

Please post some of the code.

 

PS I will be getting you code later today.

[CNCMike]

Jerry, I am not sure what you mean?

 

Cadcam, I am posting a fixture for the job we are working on. It includes a pocket cycle, drilling cycles and a tapping cycle.

 

The values are given for X and Y. A is given the value 0. In the next line of code there is a Z value that gives the initial rapid to part height along with the H1 designation.

 

See the code below.

 

N1 G20

N2 G0 G17 G40 G49 G80 G90

( 1/2 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .5 )

( CONTOUR PROFILE TOP SIDE. )

N3 T1 M6

N4 G0 G90 G54 X.01 Y-3.4899 A0. S3000 M3

N5 G43 H1 Z1.

N6 Z.1

N7 G1 Z-.125 F5.

N8 X11.99 F30

 

 

Mike

[Bill R]

A0. is the code for the fourth axis positioning. it seems like you are using the Generic Fanuc 4x mill.pst .

[CNCMike]

Bill, thanks for the suggestion. I thought I was using a 3-axis, but I may be wrong. I will double check.

 

Mike

[JerryBenoit]

Mike,

 

The Alarm you get at the machine made me wonder if the machine uses G54 work offsets or do you use just work shift with a G92?

 

If this is the case you might need to set your misc intergers to a zero (0).

[JerryBenoit]

Mike

 

Ps.

 

This is from the Generic Fanuc 3X post

 

# Misc. Values:

# --------------------------------------------------------------------------

# Integers:

#

# mi1 - Work coordinate system

# 0 = Reference return is generated and G92 with the

# X, Y and Z home positions at file head.

# 1 = Reference return is generated and G92 with the

# X, Y and Z home positions at each tool.

# 2 = WCS of G54, G55.... based on Mastercam settings.

 

 

So if you set the 1st Misc integers to zero it will not post G54.

[JerryBenoit]

Mike

 

Ps.

 

This is from the Generic Fanuc 3X post

 

# Misc. Values:

# --------------------------------------------------------------------------

# Integers:

#

# mi1 - Work coordinate system

# 0 = Reference return is generated and G92 with the

# X, Y and Z home positions at file head.

# 1 = Reference return is generated and G92 with the

# X, Y and Z home positions at each tool.

# 2 = WCS of G54, G55.... based on Mastercam settings.

 

 

So if you set the 1st Misc integers to zero it will not post G54.

[CNCMike]

Jerry, I am using G54 work offsets.

 

Bill, I was using the "MILL DEFAULT" post, which gave me the A in the code. I just tried the "MILL 3-AXIS VMC.MMD" and the A is gone.

 

Now, is there an easy way to change from the default to the 3-axis without having to start over?

 

Thanks for all the help! Mike

[cadcam]

Go to the Machine group in the ops manager.Then go to files.

look were it says Machine- toolpath copy.

use the replace button to pick the new machine. this will update the info and the post for you and then post.

[cadcam]

Are you trying to shorten the ops by post fewer ops at once to feed to the machine?

[CNCMike]

Cadcam, No I am not trying to shorten the ops. This is a fixture I designed and generated tool paths for in MCX2. It is a short program so it fits in our controllers memory.

 

I will try to change the machine definition and see how it goes.

 

Mike

[CNCMike]

Cadcam, It worked. I am going to run the program and see if everything works on that end with no alarms.

[CNCMike]

OK, here are two more problems I am having.

 

The tool change happens before the tool is called. If I start the program with T1 in the spindle the machine changes to which ever tool is waiting in the tool changer. If I start with T1 waiting in the tool changer, the machine performs the tool change, but then throws an alarm because it tried to call T1 which is now in the spindle.

 

If I bypass that by putting T1 in the spindle and skip past the M6 line the next tool change does the same thing. Rather than calling T2 it changes the tool then calls T2 again giving me the wrong tool in the spindle. See the code below. If I make the T1, T2, T3.... ect... on it's own line before the M6 everything works fine.

 

N1 G20

N2 G0 G17 G40 G49 G80 G90

( 1/2 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .5 )

( CONTOUR PROFILE TOP SIDE. )

N3 T1 M6

N4 G0 G90 G54 X.01 Y-3.4899 A0. S3000 M3

N5 G43 H1 Z1.

N6 Z.1

N7 G1 Z-.125 F5.

N8 X11.99 F30

 

This is not as big a problem, but the machine does not go home during the tool change. It only goes to the Z home position. This is fine on most parts, but if the tool is long or the part is tall, I will need to move the tool change postion so the tool does not contact the part during changing.

 

Any ideas? Thanks again for helping a newbie!!

 

Mike

[crazy^millman]

Going home really depends on the machine. What type of machine and what control is on the machine?

 

M06 on most machine will cause the arm to change. Might need to do /M06 so when you do have the tool in there you just turn on the block delete and when you do not you just turn it off.

 

BTW encase you do not know this / is block delete.

 

H

T

H

[BrianP.]

Some controllers require the T# and the M6 to be on different lines. We run Mori Seki's where I work and on some you can group the T# and M6 and on others you can't. It is a controller issue not a post.

[CNCMike]

Crazy^Millman, The machine is a Supermax VMC with a Fanuc OM control.

 

BrianP., I put the T# and M06 in different lines which works fine. My question now is, do I have to do this manually from here on out?

 

Mike

[cadcam]

Mike have you tried running any of my code in the machine. as the layout is different.

 

Here is the beginning of one of them.

 

N100 G00 G17 G20 G40 G80 G90

N110 G91 G28 Z0.

N120 (SEMI ROUGHS PROFILE)

N130 M08

N140 T6 M06 ( 3/4 FLAT ENDMILL)

N150 (MAX - Z2.25)

N160 (MIN - Z0.)

N170 G00 G17 G90 G54 X12.7155 Y-1.6819 S5820 M03

N180 G43 H6 Z2.25 T2

N190 Z.6