stops at layer changes

As the hedding may suggest, what i am after is, when in sheetcam you setup a layer, once that layer is completed will Mach3 stop and require the start button to be pressed. I will word it differently, I have not taken as much notice as probably I should have. What I am trying to achive is this. I will be using the routing function of my plasma machine (have done it before and has worked quite well). What I need to do is route one layer with a specific tool, once that layer is completed, change tools, reset the top of the material to suite the new tool and complete the next layer. Having the process stop for the tool (milling cutter) is crutial. I have already set up the layers in sheetcam and have done the simulations and all seems fine. I have never tried tool changes before so hense why I am asking. I am hoping that this process is quite simple and I am worring for nothing. Any help would be appreciated. Thanks in advance

You can create a code snippet that has the required code and just place it between the operations you want to stop/tool change. That same snippet can be used multiple times. The snippet can be labeled for what it is.

Thankyou for that jim.
Now what I need to know is how and where to put in this code snipet :blush:

This is an example of how I would do it. If your machine only holds one tool, then obviously the tool number and offset(G43) number will be the same. Your control may not use the G43 offset command. Also the G28 command may not apply as well. The code will have to be tailored to your control/machine, so a basic knowledge of G-Code and your machine capabilities is necessary.
LAYER EXAMPLE.job (15.5 KB)

Good morning jim1108. Yest that is what I am trying to achieve. Want the machine to stop, again at a convenient place for the tool change, do the tool change and then continue :mrgreen: . Zeroing out the tool I can just do manually so not worried about that, but what you have here is perfect. Just a stupid question, how do you put in a code snipet, and then how do you specify the position to stop. I normally set the zero zero location at the bottom left corner of the sheet (just a convenient place) so do I then set the tool change for that position. Just ran up the machine post extension today and all seemed to be OK. 2mm cut on a 48mm facing cutter at 18000rpm and up to 9m/m. Only thing I have found is that the router head is not perfectly perpendicular to the bed, oh well we can’t always be perfect. Probably why I am getting slight angle cuts on the plasma. I will need to fix that later.
Thanks again

There is no such thing as a stupid question.

First, create the code snippet like any other tool in your library (select the “G”).

Then type in whatever code you want the machine to do. In you case the position to stop will be where it is easy and safe to manually change the tool.

Label the snippet for what it is.

Now when you set up your operations, you can add the snippet (select the “G”) like any other tool and put it where you want.

You can create many different snippets for different jobs. Endless possibilities.

The snippet will stay with that particular job only unless you make it a part of your default tool list. In this case I would make this particular snippet for tool change a part of your default tool list.

Good morning jim1108. Was out all yesterday on site playing with a pilot boat and was knackered after that. Again thankyou for that I will give this a go and see what happens. Today after some breakdown completions will be routing out the first sheet of HDPE, however this one doesn’t need any tool changes. Whilst this is cutting will do as you suggested, possibly I may even get it right :cry:

Good morning jim108.
Got the job done yesterday afternoon, with out the tool change code snipet put in, but had to baby sit the machine and some stuffing around, but nevertheless it got done, so am happy with that. Reading the sheetcam book got the code snipet in the correct place to put in the cutting operation, but now here is the big question. We now have to type in some 'G’code for the machine to react to. Now I don’t need the machine to go to ‘the home’ position just to the ‘0’ ‘0’ position with the ‘Z’ axis at about 100mm. So now in the code snipet box I have to enter some ‘G’ code. I don’t understand ‘G’ code at the moment, so would it be possible if you could write out the code that I need to insert, so that I may type it in. My appologies for being such a pest and thankyou in advance. :mrgreen:

Try this:

G0 G90 Z100
X0 Y0
M0

Thankyou jim1108.
After doing some ‘educating’ utube style, that code that you have written is in ‘absolute’ mode.
This will first raise the Z to 100mm at the rapid speed, then move the ‘X’ and the ‘Y’ to the 0 0 position also at the rapid speed then pause. Now again a stupid question. Is it just that is all that is required or there is a return code back to where the next cut is to start. Now is it possible to enter some text to identify what is required, and would I put this in brackets before the code. ie
(Tool change time to 6mm end mill)
G0 G90 Z100
X0 Y0
M0

Again thankyou in advance

Yes, text can be entered. The machine will disregard anything in “()”. It is always a good idea to do a “dry run” with a new program especially if you are a little weak on g-coding. This can give you a chance to experiment.

With all that said, you really need to educate yourself with g-code. SC or any other CAM software will not always do exactly what you want without some tweaking either manually or editing in the post processor.

If this is for a tool change it is best to put the code in the tool change options (Options->job options->tool change). Put it in the ‘Run code before tool change’. The advantage of doing this is that after running the code SheetCam will move to the start of the next cut. If you use a code snippet SheetCam does not know that you have moved the machine so your snippet will have to also move back to the start (or near the start).

Gentlemen thankyou for your responses. I will attempt to resolve this issue, will let you know of the outcome :mrgreen:

Good morning Les.
I sent you a PM, I have no idea if you have received it. Can you let me know, thankyou

Good evening Les.
I have put into as specified.
(options, job options, tool change)
Tool change position
x0
y0
z100
Then run code before tool change there is
G0 G91 G28 Z0
G28 Y0
G90
M01
then run after tool change
M01

If this is all correct, then how do I enter this into the operations list sequence. As I am assuming without it in that list it will not do as require.
Again thankyou

Good evening Les.
I have put into as specified.
(options, job options, tool change)
Tool change position
x0
y0
z100
Then run code before tool change there is
G0 G91 G28 Z0
G28 Y0
G90
M01
then run after tool change
M01

If this is all correct, then how do I enter this into the ‘operations’ list sequence. As I am assuming without it in that list it will not do as require.
Again thankyou

For your application you should be able to just enter M1 in the ‘After tool change’ box. Leave the ‘Before tool change’ box empty.
When SheetCam sees a tool change it will now move to the position you have specified then run the ‘after tool chnage’ code. This will make the machine pause so you can change the tool.

If this is all correct, then how do I enter this into the ‘operations’ list sequence. As I am assuming without it in that list it will not do as require.

You don’t need to. SheetCam will automatically output the above tool change moves when it detects you need to change the tool.

Thanks Les.
Will try that possibly today with a dry run, at the moment it seem ‘just too simple’. Stupid question, how does sheetcam know when a tool change is required :question:

Good afternoon Les.
After looking at this more closely, the tool change is done in the ‘operations’ Once I select a tool for a layer, the next layer that requires a different tool, well there is your tool change. :mrgreen:
Now when the operations are done I get a yellow warning top left of the screen. When high lighted it says ‘Advanced cutting rule set’ ‘tool change’ This set has no active rules. When I double click on this it comes up with a box headed path rules. Do I do anything there :question:
I have entered as you requested in ‘options, job options, tool change’, set the tool change position as X0 Y0 Z100, left the ‘run code before tool change’ blank and entered M1 in the ‘run code after tool change’. Is there anything else that I need to do. Thanks again

It looks like you have tried setting up a path rule at some point. Go to Tools->cutting rules. Make sure ‘Always apply rule set’ is set to ‘None’. In your cut operation go to the ‘Cut path’ tab and make sure ‘Path rules’ is set to ‘None’.