Tool change

[Fastyankee]

I have a very large nest to cut with a lot of pierces. I’m wanting to change consumables half way through because there wil 1800 holes and I’m afraid one set of consumables wont make it. I find if a use pause I can’t lift the torch to change the consumables out.
What’s some of the way’s to do this.

[adbuch]

Perhaps break your file into two parts. Cut half the holes, change consumables, and then cut the remaining holes and outer perimeter (if required).
David

[Fastyankee]

I thought of doing that.

[acourtjester]

I had use the M01 pause command in the G-code to make changes in a cut run. You may need to write a code snippet to be inserted in the G-code to pause the movement and raise the torch for the change and then move back to the correct torch height to continue. Or maybe placing it at the end of a cut before the rapid to the next cut start, that way the touch off will correct any changes in torch height. Not all post processors can use the M01 you may contact Les for help with a custom post processor.

M1 code.JPG

[djreiswig]

I have a very large nest to cut with a lot of pierces. I’m wanting to change consumables half way through because there wil 1800 holes and I’m afraid one set of consumables wont make it. I find if a use pause I can’t lift the torch to change the consumables out.
What’s some of the way’s to do this.

If this is a one off deal, I would either split the job in SheetCam and run the post for each half. If you're doing this a lot on different jobs, you could probably add a pierce counter to your post and insert a stop automatically between parts. Then just hit start and continue.

[adbuch]

Both great ideas from Tom and djreiswig!!
David

[68rscamaro]

You can just stop it before a touch off, raise the torch and change the consumables then hit run from line.

[tcaudle]

Any of those methods work. There are all kinds of code snips you can insert any place in a file in SheetCAM

Breaking the nested parts into separate Operations in SheetCAM then gives you the opportunity to insert a code snip between any operation ,
So you break the job into 2 or more Operations, then do a few lines of G-code to move and change the consumables. then it will move back and touch off and keep cutting
You can insert lines of g-code between operations in SheetCAMm

So here is some code to put between two operations:
G0 X24.0Y10.0Z4 (tool change position)
M1

use any XYZ position you want to make it easy.

The first Operation will finish and turn off the torch and then the snip will run and when you hit the RESUME buitton it will start the second Operation that should start with a move tot he pierce point and then a touch off and it will start cutting again

We have semi auto tool change for routers/spindles that stop the spindle, move it to a pre-defined XYZ location , let you swap tools and then it moves over to a tool setter touch off device, resets Z zero for the new tool and moves back and keeps cutting . It all done in macros (sub-routines) .

Its not real common to have consumables change in the middle of a job.

[tcaudle]

One of the great features of SheetCAM is you have total control over HOW you want a job cut and in what order. Each operation is performed in the order it is in the list and you can drag them in the stack to change the order.
It will automatically treat each one as a new cut and does the touch-off and pierce stuff without having to program anything

I have been known to do inside detail cuts first then move out of the way and stop to let any tip ups be cleared an dfor things to cool off or you can simply just put in a long pause to let things cool and not have to hit RESUME again

[Fastyankee]

I have a very large nest to cut with a lot of pierces. I’m wanting to change consumables half way through because there wil 1800 holes and I’m afraid one set of consumables wont make it. I find if a use pause I can’t lift the torch to change the consumables out.
What’s some of the way’s to do this.

If this is a one off deal, I would either split the job in SheetCam and run the post for each half. If you're doing this a lot on different jobs, you could probably add a pierce counter to your post and insert a stop automatically between parts. Then just hit start and continue.

[Fastyankee]

How do I add a pierce counter? How do I add a pause? I'm fairly new to Sheet Cam but so far I really like how user friendly it is. I do all my engrave operations than my inside cuts and than outside cuts. But I'm not familiar with adding pauses. My machine uses Commend CNC and when I use pause on Command CNC it wont let me raise the torch. I also have the option to stop it and run from line which I don't like to do if I don't have to.

[tcaudle]

How do I add a pierce counter? How do I add a pause? I'm fairly new to Sheet Cam but so far I really like how user friendly it is. I do all my engrave operations than my inside cuts and than outside cuts. But I'm not familiar with adding pauses. My machine uses Commend CNC and when I use pause on Command CNC it wont let me raise the torch. I also have the option to stop it and run from line which I don't like to do if I don't have to.

The problem with pierce counters is how do you reset them without a manual REST control?

You need to knwo a little G-code to write code snips. All G and M codes are listed in your CNC Folder in the Menu on the CommadnCNC (Linux) machine. You will find there is a PAUSE (M1) that means the same has hitting the PAUSE screen buttion and then lets you continue with the RESUME button.

Breaking a cut fileinto multiple operations is dead simple. Just select the countours using the drag slect OR a Ctrl key left click select and use the Move to LAyer/New layer and name it. Everything in the layer ist hen assigned to an Operation. You can change any parameters you want but if you jsut use the same tool settings it breaks it up inot separate groups of cuts>

There is no built in pierce counter in CommandCNC so there is no variable to read and use but you are over thinking this. To do it that way you cant use Operations and simple logic. You would have to pause , move to a change position, move back to a new start and touch off. Since a pierce count could occur at any point you have to assume its in the middle of the file and deal with all the possible options in the code .

doing it in separate operations all of that is taken care of for you and all you have to do is specify the move tot eh change position and pause it. Once you hit RESUME it moves and start the next operation and that would always begin with a touch off and pierce cycle.

The problem with pierce counters is what do you do with the info and how automated beyond just displaying the numbers to the operator do you go? Pierce degranulation of consumables can vary quite a lot based on several factors . If you do a lot of thicker metal at higher current settings will show different wear than thin metal at lower currents and If you can vary the current and plunge rates DURING a pierce it changes again. its kinda like the "oil change" light on the newer vehicles.
It does not take into consideration what kind of oil you use or the kind of driving you do and it does not auto reset.

anyway. Using the Operations in SheetCAM is a fundamental way to control the cuts

At the very least you should break inside cuts from outside cuts into separate layers and Operations. Being able to cut sections then move and cut others , then come back, can have advantages too. I don't know if ShheetCAM has a piece stat in their Reports but I do know they have total cut distance and total time estimates ,

[Fastyankee]

How do I add a pierce counter? How do I add a pause? I'm fairly new to Sheet Cam but so far I really like how user friendly it is. I do all my engrave operations than my inside cuts and than outside cuts. But I'm not familiar with adding pauses. My machine uses Commend CNC and when I use pause on Command CNC it wont let me raise the torch. I also have the option to stop it and run from line which I don't like to do if I don't have to.

The problem with pierce counters is how do you reset them without a manual REST control?

You need to knwo a little G-code to write code snips. All G and M codes are listed in your CNC Folder in the Menu on the CommadnCNC (Linux) machine. You will find there is a PAUSE (M1) that means the same has hitting the PAUSE screen buttion and then lets you continue with the RESUME button.

Breaking a cut fileinto multiple operations is dead simple. Just select the countours using the drag slect OR a Ctrl key left click select and use the Move to LAyer/New layer and name it. Everything in the layer ist hen assigned to an Operation. You can change any parameters you want but if you jsut use the same tool settings it breaks it up inot separate groups of cuts>

There is no built in pierce counter in CommandCNC so there is no variable to read and use but you are over thinking this. To do it that way you cant use Operations and simple logic. You would have to pause , move to a change position, move back to a new start and touch off. Since a pierce count could occur at any point you have to assume its in the middle of the file and deal with all the possible options in the code .

doing it in separate operations all of that is taken care of for you and all you have to do is specify the move tot eh change position and pause it. Once you hit RESUME it moves and start the next operation and that would always begin with a touch off and pierce cycle.

The problem with pierce counters is what do you do with the info and how automated beyond just displaying the numbers to the operator do you go? Pierce degranulation of consumables can vary quite a lot based on several factors . If you do a lot of thicker metal at higher current settings will show different wear than thin metal at lower currents and If you can vary the current and plunge rates DURING a pierce it changes again. its kinda like the "oil change" light on the newer vehicles.
It does not take into consideration what kind of oil you use or the kind of driving you do and it does not auto reset.

anyway. Using the Operations in SheetCAM is a fundamental way to control the cuts

At the very least you should break inside cuts from outside cuts into separate layers and Operations. Being able to cut sections then move and cut others , then come back, can have advantages too. I don't know if ShheetCAM has a piece stat in their Reports but I do know they have total cut distance and total time estimates ,

I break all my operations into separate layers one layer for scribe if I'm doing a scribe than inside cuts than outside cuts. The deal with project is I have over 1800 holes to cut and that usually wears out consumables pretty quick on a project this big I'm pretty Shure it will need a consumable change 3/4 of the way through. I wasn't sure if I could just impute a pause in the G code I can do this in Comand CNC. I wish when I hit the pause button it would let me move the torch up. I normally only pause or stop on a M5 .I did not know the codes were listed in a folder on the Command CNC. Now I know M1is a pause so I can simply just input that before an M5.

Thank you for the help.

[Fastyankee]

I had use the M01 pause command in the G-code to make changes in a cut run. You may need to write a code snippet to be inserted in the G-code to pause the movement and raise the torch for the change and then move back to the correct torch height to continue. Or maybe placing it at the end of a cut before the rapid to the next cut start, that way the touch off will correct any changes in torch height. Not all post processors can use the M01 you may contact Les for help with a custom post processor.
M1 code.JPG

Thanks

[Fastyankee]

Any of those methods work. There are all kinds of code snips you can insert any place in a file in SheetCAM

Breaking the nested parts into separate Operations in SheetCAM then gives you the opportunity to insert a code snip between any operation ,
So you break the job into 2 or more Operations, then do a few lines of G-code to move and change the consumables. then it will move back and touch off and keep cutting
You can insert lines of g-code between operations in SheetCAMm

So here is some code to put between two operations:
G0 X24.0Y10.0Z4 (tool change position)
M1

use any XYZ position you want to make it easy.

The first Operation will finish and turn off the torch and then the snip will run and when you hit the RESUME buitton it will start the second Operation that should start with a move tot he pierce point and then a touch off and it will start cutting again

We have semi auto tool change for routers/spindles that stop the spindle, move it to a pre-defined XYZ location , let you swap tools and then it moves over to a tool setter touch off device, resets Z zero for the new tool and moves back and keeps cutting . It all done in macros (sub-routines) .

Its not real common to have consumables change in the middle of a job.

Awesome thank you