Post Processor for LinuxCNC and PlasmaC

More
11 Jun 2019 11:53 #136586 by rodw

Rod,

Your void sensing component sounds interesting, I am just worried that adding all of these components will add a lot of complexity to in my humble opinion is a system that doesn't need to be so complex.


My thinking is that complexity in the controller is OK if it makes the user experience simpler. In a perfect world the user should just load a file and cut it. The machine should look after all of the complexity in the background. Phill has not nailed void sensing in plasmac yet.

All of these components currently is just one, the plasmac.comp file. Keeping new features seperate is not a bad idea and Phill can decide if they get incorporated down the track either as a seperate component or by incorporating into the main system.

I might add that if I could also get Linuxcnc to calculate the arc radius, there would be no need to ever use sheetcam code snippets....
Now that would be cool
The following user(s) said Thank You: Grotius

Please Log in or Create an account to join the conversation.

More
11 Jun 2019 13:13 #136600 by thefabricator03
Rod,

I agree that the user experience should be simplified when possible.

One thing I like about Sheetcam is there is many settings that I can choose from to fine tune my machines cutting.

My main concern with simplifying the experience is that you loose some of the ability to make those small tweaks to some settings to dial in the cuts.

I would love to have a system where I can ask any one of my guys to go to my machine and have them cut great parts with little experience. I would say I am in a good position to help this community to get to that point as I cut steel from 1.6mm up to 25mm in thickness.

I worry though that the settings that work great for my machine wont perform the same on Rods machine or Phills machine. Grotius might be able to comment here on the ability of setting the cutting parameters for different machines and getting the same cut quality.

Please Log in or Create an account to join the conversation.

More
11 Jun 2019 14:12 #136609 by Grotius
@Rod,

I might add that if I could also get Linuxcnc to calculate the arc radius, there would be no need to ever use sheetcam code snippets....
You give me an idea to change colors in openGL.

github.com/LinuxCNC/linuxcnc/blob/master...hon/rs274/glcanon.py

Please Log in or Create an account to join the conversation.

More
11 Jun 2019 15:24 #136615 by islander261
Guys

You can control the THC enable from Gcode now using the correct code in your postgui.hal file to unlink the pins. You can even have the material file THC enabled and then drive from Gcode if desired, the only catch is you always have to drive from Gcode. Rod's adaptive feed is a little harder, the easiest way will be to use a digital pin pin to select control from Gcode and an analog pin to set the adaptive feed rate. I know how to do it by just looking at the adaptive feed signal from Gcode but can't even begin figure out how to convey the process to a new user who doesn't understand how the .hal works or the PP for their CAM. I think the question here is does Phill want the Plasmac branch to be the all singing and dancing job shop cnc plasma solution or is it for the new hobby user that has little understanding of cnc plasma cutting and even less of how to setup a post processor to work with their needed CAM solution. I think right now it is a compromise, the material tables make it easy for the newbie and hand coder while the being able to select the material from Gcode allows more advanced users the control they need at the expense of more material entries in the tables. Material table size should be a non issue for any controller capable running LinuxCNC.

'03

I believe in the past you said you had a CommandCNC controller. If I am to believe the adverts and T.C.'s BS it is the solution you are looking for. Remember CommandCNC is just a Gscreen app and can be adapted to use the plasmac component for Z axis control with little effort. From my previous adaptation of it to my THC it should take about 20 hours of coding and testing to make it work. Please post your CommandCNC .ini and .hal files. I would like to see how nice a job the proprietary configuration program does.

Phill

The THC enable entry in CandCNC's SheetCam post is to control the global enable of the THC hardware. It is checked at the start of each G1 block to synch the THC state machine. This works because the first move at the end of the pierce is always a G1 Z to the cut height and all later ones are at the same height. The PP to do all this plus support any tool you might hang on your Z axis is quite complex and not very robust.

A built in way to enable/disable the THC from Gcode is a nice feature for advanced users. The question then becomes is it done on a cut by cut basis or at any time in the cut? I think that the default for the feature needs to be no Gcode control to function automatically follows the material table entries.

I think it will be wise to leave the generation of material/cutting tables to the user. Anyone that has enough knowledge to use advanced features knows how to do test cuts to confirm cutting parameters. There is no way to anticipate all the hardware combinations that may be used in the field.

John
The following user(s) said Thank You: thefabricator03

Please Log in or Create an account to join the conversation.

More
11 Jun 2019 21:32 #136662 by islander261
Guys

As promised please find attached a minimal SheetCam PP for the plasmac branch. This PP requires matching SheetCam tool numbers and Plasmac material table numbers. Only the data from the Plasmac material table is actually used for cutting parameters. This PP will not insert random feed rate words or Z motion.

The Gcode file made by this PP has one SheetCam " feature" that I don't know how to defeat. At every tool change an extra G0 block that points to the current location will be put in the code. This is hard coded in the SheetCam tool change code because it is not effected by the modal state of the code. This will have no practical effect because the torch is already at that position and isn't cutting at the time.

Please test carefully on your system before use. I cut several sheets with tool changes but certainly didn't get to every possible corner condition. The file is ready to use once you strip the .txt extension off of the file name

John
Attachments:

Please Log in or Create an account to join the conversation.

More
12 Jun 2019 02:04 #136683 by thefabricator03


Please post your CommandCNC .ini and .hal files. I would like to see how nice a job the proprietary configuration program does.

John


John, Please see attached.
Attachments:

Please Log in or Create an account to join the conversation.

More
12 Jun 2019 02:21 #136685 by islander261
'03

Thank you, Moses does nice work. I had to reverse engineer mine, first the sim then a working one.

John

Please Log in or Create an account to join the conversation.

More
18 Jun 2019 12:18 #137182 by rodw
I've swapped some emails with Les at Sheetcam and have sent Phill some example output just to make sure its doing the right thing. In the mean time, here is a screen dump of some sheetcam cutting rules by SeanP that Islander261 has mentioned.
plasmaspider.com/viewtopic.php?f=114&t=25142&p=154172#p154172

Here is what we are generating when cutting a hole.
  M3 S69
  G1 Y2.850
  M67 E3 Q70 (70% of cut speed)
  G2 I0.000 J1.650
  M67 E3 Q0 (100% of cut speed)
  M5

So as long as I confirm thats what we are meant to do, I'll explain how to do this and we'll replicate Sean's rules the plasmac way. Its not something you can package up and install, you will need to make your own rules.

Please Log in or Create an account to join the conversation.

More
18 Jun 2019 15:03 #137189 by islander261
Rod

email sent

Don't you really want :

M67 E3 P0.7 for 70% feedrate

and

M67 E3 P1 for full feed rate?

The code for doing holes should be as I mentioned in the email, for changes in the cut that will effect blending the present one is correct.

John

Please Log in or Create an account to join the conversation.

More
18 Jun 2019 21:05 #137229 by rodw

Rod

email sent

Don't you really want :

M67 E3 P0.7 for 70% feedrate

and

M67 E3 P1 for full feed rate?

The code for doing holes should be as I mentioned in the email, for changes in the cut that will effect blending the present one is correct.

John


Yes, I thought so too about the Qn.n parameter but that was not how Phill has stated in his release notes so he must do something with it internally. I am waiting for feedback from him.

Please Log in or Create an account to join the conversation.

Moderators: phillc54
Time to create page: 0.161 seconds
Powered by Kunena Forum