Page 1 of 2
Tool changes with gang tool lathe
Posted: Fri Jan 07, 2022 2:50 pm
by BillB
Is there a way to eliminate tool change position move to (tool change location) in Intercon for use with gang tool lathe. So the after tool 1 we just go through to the next machining operation so the program runs unattended? What do I need to do to make that work?
Re: Tool changes with gang tool lathe
Posted: Fri Jan 07, 2022 2:55 pm
by cnckeith
Re: Tool changes with gang tool lathe
Posted: Fri Jan 07, 2022 3:49 pm
by tblough
When changing from front to rear tools, manually insert x and z moves (F1 Line) in Intercon to move the next tool to the proper side of the work.
Re: Tool changes with gang tool lathe
Posted: Sat Jan 08, 2022 2:24 am
by BillB
What if you set the tool change position to 0,0 Would that force the control just run the program without any pause or prompt. Or would it go to home position for fool change?
Re: Tool changes with gang tool lathe
Posted: Sat Jan 08, 2022 2:28 am
by cncsnw
The Lathe version of Intercon does not have a tool change position.
If you mean the G28 return point, X0 Z0 there means go to machine zero.
The move to the G28 position for each tool change is selectable on the Intercon Setup menu. Just set "Suppress G28 for tool change" to "Yes".
While you are at it, you can tell Intercon to leave the spindle and coolant running during tool changes.
You can suppress the wait-for-cycle-start in either of two ways:
1) Don't change tool numbers, just change offsets (e.g. T01, T02, T03)
2) Make a "cnctch.mac" file that is blank, or contains only a comment.
Re: Tool changes with gang tool lathe
Posted: Sat Jan 08, 2022 4:08 am
by BillB
cncsnw wrote: ↑Sat Jan 08, 2022 2:28 am
The Lathe version of Intercon does not have a tool change position.
If you mean the G28 return point, X0 Z0 there means go to machine zero.
The move to the G28 position for each tool change is selectable on the Intercon Setup menu. Just set "Suppress G28 for tool change" to "Yes".
While you are at it, you can tell Intercon to leave the spindle and coolant running during tool changes.
You can suppress the wait-for-cycle-start in either of two ways:
1) Don't change tool numbers, just change offsets (e.g. T01, T02, T03)
2) Make a "cnctch.mac" file that is blank, or contains only a comment.
Im not fiding "Suppress G28 for tool change" Is it in the Intercon window where you program the part? OR are you referring to the config setup pages Could you provide a screenshot?
Re: Tool changes with gang tool lathe
Posted: Sat Jan 08, 2022 9:17 am
by tblough
As Marc posted, the Suppress G28 is on the Intercon Setup menu. Inside Intercon press F9 Setup.
Page 80 of the Lathe Operator's Manual has a picture. If you supress the return to G28, YOU will be responsible for moving EACH AND EVERY tool clear of the work before a tool change.
Re: Tool changes with gang tool lathe
Posted: Mon Jan 10, 2022 4:39 am
by BillB
Guys would this document still be relevant for V12 lathe?
https://www.centroidcnc.com/dealersuppo ... ds/128.pdf
Re: Tool changes with gang tool lathe
Posted: Mon Jan 10, 2022 12:13 pm
by cncsnw
Pretty much.
On a Windows CNC11/CNC12 system, the tool-change macro file is c:\cnct\cnctch.mac.
The cnctch.mac file should not contain an M99. It should just be blank, or contain only a comment such as "; gang tooling -- no action required".
I am not certain you even need to set Parameter 6 = 1. You could try it both ways.
Re: Tool changes with gang tool lathe
Posted: Mon Jan 10, 2022 2:08 pm
by BillB
cncsnw wrote: ↑Mon Jan 10, 2022 12:13 pm
Pretty much.
On a Windows CNC11/CNC12 system, the tool-change macro file is c:\cnct\cnctch.mac.
The cnctch.mac file should not contain an M99. It should just be blank, or contain only a comment such as "; gang tooling -- no action required".
I am not certain you even need to set Parameter 6 = 1. You could try it both ways.
Ok thanks : )