Problem generating Gcode

[panchus]

Hi, I'm relatively new in the world of Mastercam and I'm having a problem that I can not solve.
When generating the G-Code, mastercam includes, at the end, these lines of code:

 G91 G30 Z0.
 G30 X0. Y0 A0.

The problem is that in my CNC it goes back to zero and it ruins my work.
If I delete it manually it works fine, but if I forget to remove it, disaster happens.

Is there any way that Mastercam does not include those lines?

 

Thanks

[Leon82]

Yes

 

It could be a misc integer or in the post itself

 

After every tool or just the end of the program?

Could be in the peof block or pretract block

[panchus]

Helo Leon82. Thanks for the reply.

it only appears at the end of the gCode example:

N790 X225.917 Y365.745
N792 X29.716
N794 G3 X26.716 Y362.745 I0. J-3.
N796 G1 Y31.464
N798 G0 Z25.
N800 M5
N802 G91 G30 Z0.
N804 G30 X0. Y0. A0.
N806 M30

 

 

[neurosis]

11 minutes ago, panchus said:

Helo Leon82. Thanks for the reply.

it only appears at the end of the gCode example:

N790 X225.917 Y365.745
N792 X29.716
N794 G3 X26.716 Y362.745 I0. J-3.
N796 G1 Y31.464
N798 G0 Z25.
N800 M5
N802 G91 G30 Z0.
N804 G30 X0. Y0. A0.
N806 M30

 

 

 

Do you have any experience editing your post?

[crazy^millman]

Should be a switch to change from G30 to G28. Have you tried changing it from G30 to G28 and see if it runs? That is a needed section of code and I would be very careful making some major changes.

[panchus]

Yes, I changed that value, but I thought it was not the right way to do it. I have not tried it yet,

I will.

Thank you.

[pullo]

looks like it's hard coded text  i.e . written "as is" in your post processor  in a section called peof$ (program end of file ) 

peof$

.......

      n$,  "G91 G30 Z0.". e$
     n$, " G30 X0. Y0. A0.", e$

.........

just add # in front of  these two lines  to change them  into comments like this :

 #n$,  "G91 G30 Z0.". e$ 
 #n$, " G30 X0. Y0. A0.", e$

 

Gracjan

[crazy^millman]

4 hours ago, pullo said:

looks like it's hard coded text  i.e . written "as is" in your post processor  in a section called peof$ (program end of file ) 

peof$

.......

      n$,  "G91 G30 Z0.". e$
     n$, " G30 X0. Y0. A0.", e$

.........

just add # in front of  these two lines  to change them  into comments like this :

 #n$,  "G91 G30 Z0.". e$ 
 #n$, " G30 X0. Y0. A0.", e$

 

Gracjan

Sir I would not recommend that approach. At the end of every program I have written for the last 30 years there has been some code to send the machine home to be safe 99% of the time. Yes been times when I was running production at 11 seconds a part run time I was not sending the machine home, but that was 25+ years ago.  I was ruining one tool and I was bring it up 1.0 inch and back 6.0 inch behind the vice and swapping parts every 11 seconds. Maybe I can count on my finger the others. A g28 or a G30 should always be a good code on just about any machine I have ever run. If not one then the other.

[Leon82]

The other thing can be that the 2nd return position in the machine is set  wrong.

Normally g30 can be a pallet change position, tool change position of any position you set into the parameters

 

Z is probably set to a large negative value

[pullo]

On 3/8/2018 at 3:48 PM, panchus said:

Hi, I'm relatively new in the world of Mastercam and I'm having a problem that I can not solve.
When generating the G-Code, mastercam includes, at the end, these lines of code:

 G91 G30 Z0.
 G30 X0. Y0 A0.

The problem is that in my CNC it goes back to zero and it ruins my work.
If I delete it manually it works fine, but if I forget to remove it, disaster happens.

Is there any way that Mastercam does not include those lines?

 

Thanks

I believe  that  panchus wanted to get rid of those  lines  instead of deleting them manually (IF HE REMEMBERS TO DO THAT ).  

I did  not comment as to what should be at the end of an NC-program....

Gracjan

[crazy^millman]

On 3/8/2018 at 6:13 AM, panchus said:

Helo Leon82. Thanks for the reply.

it only appears at the end of the gCode example:

N790 X225.917 Y365.745
N792 X29.716
N794 G3 X26.716 Y362.745 I0. J-3.
N796 G1 Y31.464
N798 G0 Z25.
N800 M5
N802 G91 G30 Z0.
N804 G30 X0. Y0. A0.
N806 M30

 

 

Here he says at the end so where I made my comment from. I see an M30 and that is the end of most programs so I also used that to determine my answer. 🤓🤓

[Leon82]

I would also try it with a G 91 added to that second G30 line. I think I've seen these things do some weird stuff when it wasn't specified in each line