Added a ATC to my Tormach mach3 how to add ATC in V23?

[two4tom]

Hi

I added a ATC to my Tormach 1100 with Mach3 and did a bobcad V23mill cad/cam program dry run. But in the post M1 is still in the post. I dont see in the post processor to change this? At the tool change it keeps wanting me to hit the mouse botton for the tool change.

Tom

[Joe S.]

Hi Tom,
I am not real familiar with Mach3, and I know you can edit the post processor to do what you ask, because my post Processors for Fadal and HAAS are different (the fadal does not add m1) . . . my question is , is there no method in Mach3 to enable/disable the optional stop ? Strike that question, I just looked at Mach3 screen and there is, so why not just turn it off? Anyway I think this is the line you need to comment out:
n,optional_stop just make it "n,optional_stop"

[LeeWay]

On the General Config screen in Mach 3, you have a choice of how you want Mach to handle tool changes.
Check the auto tool changer there.

[hanover owing]

thers a box rite on the program screan m1 optional stop i wouldnt recomend removing the m1 comand from your post because somtimes you may want the program to stop at the tool change i quit often inable the m1 optional stop because i need to leave the shop and and im running a part for the first time and need to watch each tool for a bit any way just check the m1 optionnal stop box and it will egnore the m1

[shred]

Change the "Tool Change" section in your POST.

Mine looks like this (I have an 1100 with the Tormach ATC). Not pretty, but it works more or less (you'll need to edit the startup code to match as well):

3. Tool change 
" "
 comment_start,"NEXT CUT - NEXT TOOL"comment_end
 system_comment
 feature_name_comment

  n,rapid_move,"G53 Z-2",coolant_off, spindle_off

   n_forced,t,"M06"," G43",h
   n,s,spindle_on, coolant_on
n,absolute_coord,work_coord
n,rapid_move,force_x,xr,yr,rotary_xy_angle

n,rapid_move," ",length_offset
output_rotary_angle
" "

You can leave the M01's in and switch them off if you want.

[LeeWay]

What I do is pretty easy though. No post changing or anything. I just have a Mach 3 profile labelled Auto Tool and another Labeled Manual Tool. I load the profile I need. The only difference in the two is that is switched in the General Config.
Load any of my code and it will do one or the other based on the profile I load. This keeps it all very simple.

[shred]

What I do is pretty easy though. No post changing or anything. I just have a Mach 3 profile labelled Auto Tool and another Labeled Manual Tool. I load the profile I need. The only difference in the two is that is switched in the General Config.
Load any of my code and it will do one or the other based on the profile I load. This keeps it all very simple.

When do you need to switch profiles? I just use the one as the ATC will ask me to put them in and take them out manually if they aren't in the carousel. Early on I tried two Mach icons that loaded different setups, but that was a mistake..

There is also now a 'disable ATC' button I saw in the Tormach Series 3 screens, but I've not tried it yet so couldn't say what it does.

[LeeWay]

One part I make does engraving and spotting for drilling as well as milling out some holes with the mill drill.
It's all the same tool, but I have to tell it differently in Cam, so it acts like three tools to Mach. That profile is Auto Tool Changer.
Other parts I make I have to manually swap tools. The other profile allows that.
When I open Mach 3, it flashes a screen with all my profiles on it. I select the one I need and it loads up.

[FRITZ W.]

Take a look at this file from Tormach on ATC machine control software. It may be what you are looking for.

Direct Document and Software Download | Tormach LLC | We provide personal small CNC machines, CNC tooling, and many more CNC items

Can't get the link to post correctly but it does work it you just copy and paste.

Take care,
Fritz