Trouble with G54 and tool height compensation

[stefano.oteri]

Good morning,
We need to carry out the zeroing process of the piece (i.e. G54) and the adjustment of the height of the tool (i.e. H01 for tool T01) when starting each single processing, because, when performing two consecutive works with the same tool, these parameters are not inserted automatically during the second work. In case of restart of the second work, the processing coordinates would go lost.
How is it possible to solve this issue?
Thank you

[seth.madore]

When you say "the second work", do you mean a second work piece (G55), or the second operation of a tool?

What is your control, and what is your post processor?

[stefano.oteri]

I mean second operation of a tool, my control is fanuc and my post processor is Doosan 3/5-axis VMC (FANUC) preset.

Thank you

[seth.madore]

And is your machine and control also a Doosan mill?

[seth.madore]

Take a look at the Haas NGC post, there's an option for "Safe Start all operations", which gives us this between operations:

N125 G1 X-8.1
N130 G3 X-8.125 Y-0.6535 I0. J-0.025
N135 G1 G40 X-8.125 Y-0.6785
N140 G0 Z0.1

(Face1)
/ N145 G53 G0 Z0.
/ N150 T1 M6
N155 S4750 M3
/ N160 G154 P4
/ N165 M8
/ N170 G1 X0.3 Y-0.2437 F650.
/ N175 G0 G43 Z0.1 H51
N180 G1 X0.3 Y-0.2437 F650.
/ N185 T2

[stefano.oteri]

Yes, we have doosan mill. Is it possible to add this option that we are using to the post processor? Because we have already customized some things and this would be all we need to be performing.

Thank you

[seth.madore · Accepted solution]

Yes, it's possible to add that functionality to the Doosan mill/turn post, but it's not a quick copy/paste, as there are about 17 sections of code that need to be carried over from one post to the next. This is something you can either: 1) attempt to do on your own, with the forums as "help", or 2) reach out to one of our channel partners and have them do it for you

[programming2C78B]

I don't know what the equivalent is, but there should be a "program restart" setting on the machine that has to be turned on. 

[stefano.oteri]

So, are you saying there is a button that can reactivate the data we need and can restart works from that point? Please can you tell us which button?

Thank you

[Eric_E · Accepted solution]

You can add operation in your tool path browser - (right click select new operation, Manual NC, for manual type select "Force tool change"), place this before the second instance of the tool you want to be able to re-start. this way you should not have to edit your post processor.