Repeat Cutting?

[Bruce]

I am doing a project that is using 120 sheets of materail... the same thing is being cut out of each sheet of material... one bit, same tool path for each sheet.
I have a Panther with the FTC so I know I can just repeat the job after a new sheet is ready to go without having to re-enter the file, but is there a way where I can bypass the bit having to measure itself each time since there is no need for it to do this? It'd save a lot of time. This would also be useful on other jobs I do that are repeat of the same cut with no bit change.

Thanks!

[ArtFab]

On my Stinger II, I routinely use both the CAMaster Single tool Inch post processor and the CAMaster ToolChange Inch post processor. I pre measure the tool and I use the CAMaster Single tool Inch post processor when saving the tool path to avoid the tool being measured when the file is run.

[Charlie_L]

Bruce,
Given 120 sheets, you might even want to add a few lines of code to your tap file that move the spindle out of the way. I sometimes also modify it so that the spindle stays running, especially if the run is short and there are many sheets to cut. Obviously, you have to worry about the safety of the spinning bit and how it might be accidentally come in contact with.

[Bruce]

Thanks for the recommendations... even though I've had the machine 3+ years, I'm not familiar with adding code to the tap file.. that's one for youtube that I'll look up. Same with the single inch tool post processor.. not sure on the "pre-measure" where to measure from, etc.

Aside from straight vcarve coding, I have extended my knowledge beyond this.

Kind Regards,
Bruce

[james mcgrew]

Bruce in the tap file is a command to do the recalc tool, if it is removed the file will operate with out it. Send me your INI ans macro file and the tap file and i will do this. or later today you can call and we can do this online

Just let me know Jim

[Charlie_L]

Bruce,
Maybe this would get you started if you want to try....

Make two copies of your normal TAP file. Give them names so you know which one includes the tool measure FTC function.

Use the FTC file to cut the first sheet.

Then, in file manager we will open the second file that will be cutting the remaining 119 sheets.
Hover over this file name and Right click. Select the "Open With" command and choose "Notepad" to open this file.

Inside you will find something like this near the beginning of the file.
----------------------
N2 G90
N3
N4 M5
N5 G53 Z0
N6
N7 [5075 45/15 Veining Bit]
N8 T1 [ GET TOOL NUMBER 1 ]
N9
N10 S12000 [ SET SPINDLE SPEED RPM ]
N11 M3 [SPINDLE ON]
N12
N13 G00 X0.000 Y0.000
N14 G53 Z0
N15
------------------------

On the row having the tool change, in this example "T1" we are going to add one character, a square bracket "[" as shown below. I made it bold just so it easier to see.
N8 [T1 [ GET TOOL NUMBER 1 ]

Next, save this change and you are ready to go.

The square bracket comments out the line of code so WinCNC will ignore everything on that line.

Don't worry about the N8, N9, N10 etc.... Those are simply row numbers and are not important.

[Bruce]

Thanks for all the info and help.. Jim, if I can give you a call on Monday, that would be great.. PM me a time that works best.
Charlie, I'll give your recommendation a try...

Kind Regards,
Bruce

[Bruce]

Thanks Charlie, that worked perfectly... a big time saver and I'll definitely use it in the future as well.
Is there a website that has different coding that I can learn from? Such as to have the machine move to a certain area when it's finished with the toolpath. I've done HTML work in the past so I'm familiar with changing code, etc but just have to know where to go to find it.

Again, this forum and the people here are one of the reasons I went with Camaster. I had ZERO experience when I purchased my machine and though I probably use 10% of what it can do, I'm always picking up tips here. Thank you all!

[rcrawford]

Read the WinCNC manual. There is a list of all the G-code.

At the end of your file, you will see a line that has G53Z on it (raises the spindle as high as it will go). And then an M5 (turn spindle off). Hit enter after that line to create a new line, and type in G00 X0Y96 (or whatever XY you want it to move to at the end of the file).

[james mcgrew]

This can be done in a macro (I have specific places for end of file and Park) do not change this without some help from someone who is familiar to this.

Always and right now make a copy of the entire wincnc folder that is on the c drive under programs DO THIS NOW if you have not already

[Bruce]

Thanks Jim.. at this point I'll leave enough alone since just having not to measure the bit each time is a big time saver. I do have all my files backed up but not the wincnc folder so that will be done tomorrow.