Hi
I have a 3Axis mill with a Fagor 8055 controller.
I am a newbie and trying to write G-Code to rotate a profile.
The profile is a 3D path of 450 lines which needs to be passed along 12 times at 1mm Z levels.
Rather then duplicate the profile 12 times with corrected Z figures, I want to repeat the profile and alter the Z level.
Can this be done by altering the Tool Length Compensation.
This is a sample of what I have (may be all wrong):
Many Thanks
Kiwi.

N100 (IF(P1 EQ -1)P1 = -2) ;??
(IF(P1 EQ 0)P1 = -1) ;??
N200 G00 X0 Y0 Z15
G43 ZP1 ;?? Set Z Compensation
;(Start of Path)
G01 X0 Y0 Z0 ;Sample Only
X20 Y5 Z-7 ;Sample Only
X30 Y8 Z-12 ;Sample Only
;(End of Path)
N400 G00 Z15
X0 Y0
(RPT N100, N400) N3
G44 ;?? Canel Z Compensation
N500 G73 Q10
(RPT N100, N500) N3

How about showing us a sketch and the code you have
so we can better understand.
PEACE:D

Hi Hardmill, Thanks,

Shortened version.

JPEG & Txt files attached.

Regards
Kiwi

Suggest.
Make a loop.
Set #1=0 (Loop counter)
Set #2=1 (Cutting depth)
While #1 LE 12 DO 1 (Something like this, not sure)
your countour comes here, and change all your Z levels to
Z[your value - #2]
#1=#1+1
End loop

Not sure about the exaxtly typing, have to look in the manual for that.

What do you think? could it work.

Per

Hi Per_N,

Thankyou for your reply.
If I understand you correctly, your solution is stepping the Z value in increments to the value of #2?
If this is correct, I don't think that is what I need.
My problem is that this is a 3D profile, and the Z value is changing along the path.
I have found that my controller has a Zero Offset Table with Codes G58 & G59. I am still trying to find out if this is my answer.
If someone know a little about these codes I would appreciate any advise.

Regards
Kiwi
NZ

Kiwi-

My machine uses these codes...incremental offsets (both G58 and G59). If you're looking to repeat the same program you'd change it to:
(ORGX58=?,ORGY58=?,ORGZ58=?) The ?s being the incremental moves...if you're looking to move the part over 1" in X only and repeat the program with a deeper Z depth of, say, .25 you'd change it to:
(ORGX58=1,ORGY58=0,ORGZ58=-.25)
G58
(RPT N100,N400)

Hope that helps.

Jen

Hi Jen,

Thankyou for your help, this looks like what I'm looking for.

Earlier today I changed the Z setting in the Zero Offset Table under G58 from 0 to -2(mm) , but when I run the program it stops with a warning...over riding the soft limits.

I've had another read of the manual and it covers the (ORGZ 58=?) that you refer to.
I'll study this further and have another go tomorrow.

Regards
Kiwi
NZ.

If i get your question right, you wan't to repeat the same path a number of times. But change only the Z value. If this is correct the my loop will work perfectly if you understand what I ment.

Regards Per

If all you are wanting to do is run the exact same toolpath with a different tool length, try using the G10 command. You can incrementally change your tool length compensation by using:
G10G91L?P?Z-.1 ect
Check your manual to see what "L" you need for tool offsets (usually L10) and "P" will be the tool offset number.

Hi Per_N

My understanding from the code you supplied is that the Z value is constant for each pass. Correct me if I'm wrong.
I need the Z value to change as this is a 3D profile.
I want to make each pass 1mm deeper then the previous pass.

Thank you for your help.
Regards
Kiwi.

Hi E_Stop,

Thankyou for your help.
After trying to use (ORGZ 58=?) without any success, I now think your suggestion may be the answer.
Your G-Code must have some variations to what I use as G10 command for my controller is 'Mirror Image Cancellation'.
G43 is Tool Length Compensation which I am still trying is get to work.

Regards
Kiwi.

Hi Jen,

Tried (ORGZ 58=?) but this appears to relate to the HOME Zero on my machine. Every time I ran the code I would lose my settings and it would run under the Home references.
This may be a factory setting?

Regards
Kiwi

Originally posted by Kiwi

G43 is Tool Length Compensation which I am still trying is get to work.


KIWI--

G43 is typically a call for the Tool Length Compensation. So, G43 H1 blah blah blah just tells it to use the tool compensation amount in offset #1. The G10 that I referred to modifies the value in the offset so that the next time G43 calls for it, it will have changed by the 1mm you need.

Kiwi-
You need to put in the part zero (G54) for the G58 to reference. I didn't look at your program before, sorry. Also, you're missing the G43 which should go after the T1 M6. I have the 8055 M controller - you shouldn't have to put in a D or H value...I'll send you a PM with one of my programs so you can get an idea of the layout.

Jen

Your wrong. The Z path would be change the amount that you put in the #2. But I see that I have forgotten one thing, you also have to put in third parameter that keeps track of the previos cut.
Like #3=#3+#2

I take this one more time.
#1=15 (Number of cuts)
#2=2 (cutting depth in each cut)
#3=0 (counter where we are)
#10=0 (Loop counter)
WHILE #10 LE #1 DO1
G0 X0. Y0. (STARTPOINT OF PATH)
G1 Z[0 - #3]
X20. Y5. Z[-7. -#3]
X30. Y8. Z[-12 -#3]
G0Z1.
#3=#3+#2
#10=#10+1
G0 X0. Y0.
END1
G0 Z10. (AFTER 15 CUTS THE PROG. WILL CONTINUE HERE

I hope you understand this.
This is how I should do in a Fanuc control, I don't now what Fadal have but I think they have Fanuc too or?

Regards Per

Hi Per_N

Thanks for the explanation.
I'll need to study this further as my controller is a FAGOR and I suspect the code may vary?

Regards Kiwi

Hi again Per_N

On further examination of your code I don't think this is a practical solution to my problem as I have about 450 blocks of code and if each one with a Z value needs to be modified to Z(-?-#3).
I can copy the profile code 12 times and I have a macro that can add the increments to the Z values but considered this a clumsy way.

Thankyou for your help.
Regards
Kiwi

Have you ever heard of something could Nc-Editor or change of postprocessor.

I don't want to be rood, but this is Sunday school programming.
Study the manual some more before you get into to this type of programming.

Good luck to you.

Per

Per_N

Thankyou for your help and advice.

Kiwi.