Problem- canned cycle cannot perform positive value ??

[xray34]

Hi,

I did this part in Edgecam V9.5 and everything works except 1 line in the nc file.

On line 'N2051' my Hurco says
'CANNOT PERFORM A CANNED CYCLE WITH A POSITIVE VALUE'

Can anyone shed some light on why this has happened?

Edgecam showed everything ok and simulated machining perfectly.

attached is a txt file of the NC code .

Need to start producing this part monday am...

Thanks for any help people. :-)

[glovebox20]

Hello

N2046 M25
N2047 T1 M06
N2048 S2000 M3 M8
N2049 G0 X-12.59 Y49.22 M8
N2050 Z5.0
N2051 G98 G81 Z-3.0 R2.0 F200.0 H01
N2052 G90
N2053 X0.0 Y-50.8
N2054 G80

This is not the format that I run on the VMX that I'm familiar with. The Format That I use goes something Like This:

M25 Home Z-axis
T1 M06 Change Tools
S2000 M3 Spindle on
G90 G0 X-12.59 Y49.22 M8 Position Table in X,Y, Coolant On
Z30.0 Brings Tool 30.0 above Part
Z1.0 Brings Tool 1.0 above Part
G81 X-12.59 Y49.22 Z4.0 F200.0 Spot Drill 4.0 down from start (or -3.0 from Z0)
G80 Z30.0 Canned Cycle cancle, Tool 30.0 above part
X0.0 Y-50.8 Position table
Z1.0 Brings Tool 1.0 above part
G81 X0.0 Y-50.8 Z4.0 F200.0 Spot Drill again
G80 Z30.0 Canned cycle cancel, Z 30.0 above part
M9 Coolant off
M25 Home Z axis
T34 M06 Tool change


I believe Hurco's use "Basic NC" code for their G code Side. Which basically means that their Canned cycles are Incremental movements on Z unlike the Standard Fanuc Format. Also, All Z values are positive but the Drill still goes in the negative direction. So it get a bit clumsy to work with. Let's try it again with a Peck Drill cycle


M25 Home Z-axis
T2 M06 Change Tools
S2000 M3 Spindle on
G90 G0 X-12.59 Y49.22 M8 Position Table in X,Y, Coolant On
Z30.0 Brings Tool 30.0 above Part
Z1.0 Brings Tool 1.0 above Part
G83 X-12.59 Y49.22 Z21. Z4.0 F200.0 Peck Drill 21.0 down from start (or -20.0 from Z0) with a Peck of 4.0 (Second Z is the Peck amount)
G80 Z30.0 Canned Cycle cancel, Tool 30.0 above part
X0.0 Y-50.8 Position table
Z1.0 Brings Tool 1.0 above part
G83 X0.0 Y-50.8 Z21. Z4.0 F200.0 Peck Drill drill again
G80 Z30.0 Canned cycle cancel, Z 30.0 above part
M9 Coolant off
M25 Home Z axis
T34 M06 Tool change

I believe Hurco's do have the OPTION to run Industry Standard NC (ISNC) so it would be Fanuc compatible. But It's an OPTION and it must be installed on YOUR machine to use it.

Hope this helps
glovbox20

[xray34]

Thanks SO MUCH 'glovebox20'

As you can prob tell I'm still learning NC code and things like canned cycles cause me porblems and the errors are difficult to see.
Edgcam has so far been good to me but I will be happier when I'm more conversant with the codes.

Thanks again for your help, you have made my monday a lot easier now.
Respect

xray34

[CNCRim]

Don't rely too much on CAD/CAM unless you know or very riable post processor.

[xray34]

Good point 'CNCRim'...

This is why I'm trying to learn NC programming as quick as I can
and with all the knowledge on this forum I'm sure
I will learn fairly quickly.

Thanks man.

Respect :-)

Originally Posted by CNCRim Don't rely too much on CAD/CAM unless you know or very riable post processor.

[xray34]

The part was made this morning and your code fix for me worked perfectly.
Its something I will now always remember..

Thanks again 'glovebox20'

xray34

[glovebox20]

Happy to help.

Just don't be afraid to correct me if I'm wrong.

glovebox20

[Rally]

Originally Posted by glovebox20 Happy to help. Just don't be afraid to correct me if I'm wrong. glovebox20

You are wrong

[Rally]

HA HA just kidding that info helped me as well
Thanks