Parking

[rwskinner]

In Sheetcam, why can't there be an option in parking for absolute machine coordinates instead of work coordinates?
Wouldn't be as simple as adding a G53 on the same line as the Xand Y parking position?

Are the parking position variables exposed in the post so we can edit our own method?

Richard

[acourtjester]

This may not be what you are looking for but you could write a G-code for positioning before loading the cut G-code.
Meaning home your table then have a G-code to move X and Y to the coordinates you want and then have G92X0.0Y0.0 as the last line. then load your cut G-code which is set to start at X0.0 Y0.0

[rwskinner]

I imagine the reason parking and load material comes using work offsets is that many folks do not have home switches on their cnc plasma tables. I fixed several little items in the CandCNC Screen set such as the button script for Load Material to utilize the G53 Machine Coordinates so it "always" goes to the same known location, which is how most cnc machines operate, at least all of mine. I think I have fixed it by entering the code I wanted in the post OnFinish and Not setting X&Y back to zero and it should do as intended but I'm not out there right now.

I didn't actually see where the parking code was in the post, so I imagine those are done behind the scenes and that is why it's not shown. I guess another way to handle it is to have the post put a custom macro in the G-Code onFinish and then that Mach3 macro can do anything you want the machine to do.

It just seems too easy in the Sheetcam config to have a checkbox for using absolute machine coordinates so users have a choice. When you post the G-Code, insert the G53 on the same line as the coordinates. Since it will only be used for the commands on the same line. As a quick example:
G53 G00 Z2.5 'Raise Z up first
G53 G00 X ParkPosX Y ParkPosY 'Move to Park Position

This eliminates people crashing there machines because there work Zero is now in the middle of a sheet. Maybe I'm making too much of it but it's just feels strange having all the machines act a certain way while one is an odd ball.

[Les Newell]

In the next development version there will be an option to add your own custom parking code. I don't know why I didn't add this sooner.
As a workaround until that version is released you could modify your post processor to always park. Go to Options->machine->post processor and click on the 'edit post' button. Look for

Code: Select all

function OnFinish()

The code in there will vary depending on the post you are using but hopefully it should be fairly obvious where you need to add the parking code. This code will do the parking moves:

Code: Select all

   post.Text(" G53 G00 Z2.5\n")
   post.Text(" G53 G00 X0 Y0\n")

If you have any trouble let me know what post you are using and I'll give you exact instructions on how to change it.

[rwskinner]

I upgraded to 6.0.19 and still didn't see the option. Where is it located?

It would be kind of cool to have custom code to be inserted before and/or after a job, kind of like you have for tool change.

So if I want to Got into Exact Stop Mode I could enter that into the Start Section, or Goto X0Y0 Z2.5 then M3 to prefire the torch and blow water off or precharge the air on the torch.

Custom code before the M30 could do anything I wanted, like move the machine to it's parking position, Or Lift Up 2.5" and wait there till post flow turned off then move to parking position so it doesn't blow water everywhere.

Crazy Examples I know. Maybe we can do it now and I just don't know how.

Richard

[Les Newell]

Parking code is only in the development version (V6.1.x series), not the stable version (V6.0.x series). You can install both versions on your computer at the same time if you wish to try it.

For custom code you can use the 'insert g-code' operation. This allows you to add g-code anywhere you want. The only thing to be aware of is that SheetCam does not try to work out what your gcode is doing. If you change coordinate systems or move the Z axis below the top of the work SheetCam won't know you have done it.