Gcode pause utility

[Mr.Chips]

I was looking at some pause questions back in 2008 and the answer was that Cut3D didn't support one.

I am looking at running some files that would take 40 plus hours so I need a way to pause or shut down and restart the file without damaging the work is there currently a way?
Thanks

[Adrian]

That's a facility that should be part of your control software (Mach3, WinCNC, SB3 etc) rather than Cut3D.

Which one are you using?

[tmerrill]

I am looking at running some files that would take 40 plus hours

You may also want to ensure (ask) whether you have set the files up correctly as 40 hours is a long time even for a 3D Finish toolpath.

Also, if you are using the time estimate provided in Cut3D, have you set the Rapid Rate and calibrated the scale factor for your machine? You may be making decisions based on an incorrect time estimate.

Tim

[Mr.Chips]

That's a facility that should be part of your control software (Mach3, WinCNC, SB3 etc) rather than Cut3D.

Which one are you using?

I'm using Mach3 inches

Thanks

[Mr.Chips]

I am looking at running some files that would take 40 plus hours

You may also want to ensure (ask) whether you have set the files up correctly as 40 hours is a long time even for a 3D Finish toolpath.

Also, if you are using the time estimate provided in Cut3D, have you set the Rapid Rate and calibrated the scale factor for your machine? You may be making decisions based on an incorrect time estimate.

Tim

The cut area is 20" x 62". finish cut at 80 IPM at 7% step over, 1/8" RN bit, it will take approx. 46-1/2 hours of cutting.

I cut a sample 11x12" and the finish cut was 2.5 hr. excellent finish.

[mrmfwilson]

Seems like a really long time to cut something to me also. I use a special Mach 3 screen that is built by the machine manufacturer. My screen is set up with a "Run From" button. It allows you to run the file from a specific line. Not familiar with the standard Mach screen but there should be a way to do this with the standard screen. Make sure and save the offset setting with the Config > Fixtures... You could pause the machine and jot down the line number. Shut down the machine. Restart the machine the next day. Home the machine if necessary and restart the cutting from the last line number that you wrote down.

Mike

[PaulRowntree]

This is trivial if you have accurate homing switches, since accidental movement when powered off would be removed when you re-home the machine.

[tmerrill]

Hager,

Here is a possible solution:

I believe you also have VCarve Pro based on your previous posts. If so, you can import your Cut3D toolpaths into VCP and either use Tape Splitting or Tile Toolpaths to break the file up into smaller pieces.

Tape Splitting is a modification you would make to your VCP post processor (note it is not supported by Cut3D) and it is explained in the Post Processor editing guide found under the Help pull down menu.

Tile Toolpaths is typically used to machine a project larger than your machine bed, however in this case you would be moving your X,Y origin point instead of the material. There is a tutorial in the support materials section if you aren't familiar with the concept.

Tim

[Mr.Chips]

Hager,

Here is a possible solution:

I believe you also have VCarve Pro based on your previous posts. If so, you can import your Cut3D toolpaths into VCP and either use Tape Splitting or Tile Toolpaths to break the file up into smaller pieces.

Tape Splitting is a modification you would make to your VCP post processor (note it is not supported by Cut3D) and it is explained in the Post Processor editing guide found under the Help pull down menu.

Tile Toolpaths is typically used to machine a project larger than your machine bed, however in this case you would be moving your X,Y origin point instead of the material. There is a tutorial in the support materials section if you aren't familiar with the concept.

Tim

Thanks Tim,
I will look into the Tape Splitting that sounds like a good way to go.

I will do a lot of studying before I start this as well as some sample runs.

Also considering rather than cutting the entire surface just make a irregular shape around the subject to still look nice but gratly reduce the cut times. Least that's an option.

Thanks you all your comments.

[tmerrill]

One word of caution here. Wood being wood, any lengthy pause can allow wood movement and when you pickup where you left off, especially with a detailed 3D finish pass, you can end up with a ridge or groove. It may only be a couple of thousandths but depending on the location in the model it can be noticeable and take time to blend in. There are so many variables there is no way to predict when it may happen but I've seen it approximately 1/3 of the time and I use tape splitting often during our afternoon thunderstorm season.

Tim

[Leo]

The run from here in Mach3 works well. There are a couple of steps to get used to but it is fine.

I have also taken a really long program and divided the actual CNC program into sections.
There should be plenty of places in the program where the cutter gets to a .1 - or some place above the part.
Even if not - you can insert g-code to move the cutter where ever you want it to go.
What I did was to save the program and divide it up in places I wanted then wrote the g-code to bring the cutter back into the cut "gently".
Yes - I have been writing g-code for 30 plus years - so this is not an issue to me.
YES - with a little thought - it is pretty easy to do.
YES - ABSOLUTELY - run SLOW - be CAREFUL.

One of the nice things about Aspire is to be able ti "tile" or to cut sections at a time.

YES - WOOD - MOVES.
If you do a section then come back tomorrow to finish - it probably moved.
In face - is can move DURING - a long operation
NO - there is nothing you can do to stop the movement

[rscrawford]

Tim makes a great point. You are releasing tension in the wood when you carve out one side. Then leave it sitting overnight and it will definitely move (warp, twist, bow, etc).

What machine are you using? 80ipm seems slow for a 7% stepover finish, unless that is all your machine will handle. If you have a sturdy machine I'd bump that up as high as possible. There will be no force from the actual cut (you are taking off .00875"/pass), so its just the forces from moving the spindle you need to worry about. On my Cobra, I'd set xy feedrate to 600ipm, and z to 400ipm.

[Mr.Chips]

The run from here in Mach3 works well. There are a couple of steps to get used to but it is fine.

I have also taken a really long program and divided the actual CNC program into sections.
There should be plenty of places in the program where the cutter gets to a .1 - or some place above the part.
Even if not - you can insert g-code to move the cutter where ever you want it to go.
What I did was to save the program and divide it up in places I wanted then wrote the g-code to bring the cutter back into the cut "gently".
Yes - I have been writing g-code for 30 plus years - so this is not an issue to me.
YES - with a little thought - it is pretty easy to do.
YES - ABSOLUTELY - run SLOW - be CAREFUL.

One of the nice things about Aspire is to be able ti "tile" or to cut sections at a time.

YES - WOOD - MOVES.
If you do a section then come back tomorrow to finish - it probably moved.
In face - is can move DURING - a long operation
NO - there is nothing you can do to stop the movement

Thanks for the comments.

Can you expound on "gently"'.
On thing possibly in my favor is that the slab is three inches thick.
Hager

[Leo]

When I say gently - I mean to feed into the cut with a slower than normal feedrate and at an angle entering the cut.

This is not something that you would do in Cut3D.

[Mr.Chips]

When I say gently - I mean to feed into the cut with a slower than normal feedrate and at an angle entering the cut.

This is not something that you would do in Cut3D.

Got it.
Thanks
Hager