Need Help!- 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. :-)

[rider23]

why is there an h value on that line , should it be with the z5. line ?
and do you need a g43 on the z5. line so that it would read
g43 z5. h01

[MIKEL12]

Yes i agree, the code should look like this:

N2047 T1 M06
N2048 S2000 M3 M8
N2049 G0 G90 X-12.59 Y49.22 M8
N2050 G43 H01 Z5.0
N2051 G98 G81 Z-3.0 R2.0 F200.0

(Although i guess the G90 might be wrong in this depending on if your running inc beforehand)

[xray34]

as far as I can see the H01 seems to refer to the center drill tool location.
as lower down the code @ line N2062 there is an H34 which I assume refers to the drill I have @ location 34

I'm still learning NC code so please feel free to explain my mistakes further.

Thanks for your replies. 'rider23' 'MIKEL12'

xray34

[MIKEL12]

http://www.cncezpro.com/g43m.cfm

Basically if you write G43 H01 Z5 the tool tip will move to Z5

So the value stored (by you) at H01 in the controler is the length of the tool.
When you write G43 H01 you tell the machine that the tool is "this long".
And then when you move to Z5 you move the tooltip to Z5 and not the spindle zero.

Then the next tool you do the same thing and this way you never have to think about the tool length when programming. It will always go to Z5 (5mm above where your working coordinate system is set)

Hope this clears it up

[xray34]

Perfect thanks..

I love this forum, so much consice help.

Cheers MIKEL12

Originally Posted by MIKEL12 http://www.cncezpro.com/g43m.cfm Basically if you write G43 H01 Z5 the tool tip will move to Z5 So the value stored (by you) at H01 in the controler is the length of the tool. When you write G43 H01 you tell the machine that the tool is "this long". And then when you move to Z5 you move the tooltip to Z5 and not the spindle zero. Then the next tool you do the same thing and this way you never have to think about the tool length when programming. It will always go to Z5 (5mm above where your working coordinate system is set) Hope this clears it up

[jstikeleather]

Here is a PDF document of Hurco canned cycle parameters.

I believe you are using BNC mode on your Hurco, given the fact that your canned cycle requires positive Z values.

If you need further clarification on anything in this document please ask.

[xray34]

Thanks 'jstikeleather'