Post Processor for LinuxCNC and PlasmaC

More
05 Jun 2019 07:05 #135915 by phillc54

also agree with Tom who made a comment in another thread about having plasmac trying to do everything, A stripped down basic version would be very handy for newbies or those who dont like over complicated CAM programs. But I am hoping that in time we will have that.

You do NOT need a cam program to use plasmac, I don't have one. All the samples are hand coded with the exception of the wrench which I think was originally done for my mill with dxftogcode.

Cheers, Phill.

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

More
05 Jun 2019 07:24 #135916 by rodw

thefabricator03 wrote:
I do agree that a tutorial would be handy, But at the moment with the ongoing development of Plasmac it is not the right time to do that until it is finished.

I deleted that plasmac specific code from the post and now I can import my gcode.

I also agree with Tom who made a comment in another thread about having plasmac trying to do everything, A stripped down basic version would be very handy for newbies or those who dont like over complicated CAM programs. But I am hoping that in time we will have that.


Really, Phill's intent was to allow anybody to load up a XY gcode file, select the material and run it. But if you are like Islander, '03 and myself where you are cutting full sheets at a time, you really need the nesting features of Sheetcam. Its incredible value for the price and runs on Windows and Linux.

The "M190 Pn" was the method Phill came up with to select the Plasmac tool from Gcode. It is followed by an M66 while it waits for an acknowledgement from Plasmac to say its loaded the selected tool. If you have a lot of tools, this needs wait for longer than 1 second (I had to go to 2 seconds with 50 tools). Then you can use the plasmac feed rate if you wish using standard Hal naming conventions.

And Phill parses the gcode file and won't allow a gcode file to be loaded if there are any invalid tool numbers in it.

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

More
05 Jun 2019 08:37 #135918 by JTknives
My experance is with cnc mills and lathes so I understand diffrent tools. But how many “tools” do you need with a plasma cutter. Is each tool a diffrent thickness of material?and as such has diffrent feed rates? Or a tool specific for holes? I can see a tool just for holes being handy. The holes I cut are usaly under 1/4” and THC is not real great with that.

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

More
05 Jun 2019 08:48 - 05 Jun 2019 08:49 #135919 by rodw

JTknives wrote: My experance is with cnc mills and lathes so I understand diffrent tools. But how many “tools” do you need with a plasma cutter. Is each tool a diffrent thickness of material?and as such has diffrent feed rates? Or a tool specific for holes? I can see a tool just for holes being handy. The holes I cut are usaly under 1/4” and THC is not real great with that.


Its probably easy at 30 amps but if you have a 120 amp machine with cut charts for mild steel, stainless steel and aluminium and your machine has consumable sets for 30 amps, 40 amps, 60 amps, 80 amps, 100 amps and 120 amps plus a choice of shielded and unshielded consumables (I have not implemented unshielded) and the ability to cut thicknesses from 1 mm to 20 mm and there are multiple amperage options for a given material thickness, its not hard to get to 50 tools just from entering the manufacturer's cut charts.
Last edit: 05 Jun 2019 08:49 by rodw.

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

More
05 Jun 2019 08:53 - 05 Jun 2019 09:01 #135920 by thefabricator03

JTknives wrote: My experance is with cnc mills and lathes so I understand diffrent tools. But how many “tools” do you need with a plasma cutter. Is each tool a diffrent thickness of material?and as such has diffrent feed rates? Or a tool specific for holes? I can see a tool just for holes being handy. The holes I cut are usaly under 1/4” and THC is not real great with that.


With my CandCNC setup,

I had a tool set up in sheetcam for each thickness of material and within the thickness I had different amperages that I cut at for different size consumables.

So It went like this

1.6 sheet 45 amp
1.6 sheet Finecut
3mm sheet 45 amp
3mm sheet finecut
6mm plate 45 amp
6mm plate 65 amp
8mm plate 65 amp
8mm plate 105 amp
10mm plate 65 amps
10mm plate 105 amps
12mm plate 65 amps
12mm plate 105 amps
16mm plate 105 amps
16mm plate 125 amps
20mm plate 105 amps
20mm plate 125 amps
25mm plate 125 amps

And a drill tool set up for center marks

I would sometimes cut material with a higher amperage to increase the cutting speed if the item did not have need to have very square edges and holes.

With holes I use sheetcam rules to slow the feed rate down to 60% of normal rate for that tool.
Last edit: 05 Jun 2019 09:01 by thefabricator03.

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

More
05 Jun 2019 10:00 - 05 Jun 2019 10:02 #135922 by rodw

thefabricator03 wrote:
With holes I use sheetcam rules to slow the feed rate down to 60% of normal rate for that tool.


In theory this should work just by changing the feed rate as the cornerlock feature of plasmac should kick in without the need to disable the THC from G code.

In fact you prompted me to look something up. One issue with Sheetcam hole rules with plasmac is that plasmac is the master of feed rates so there is no guarantee that sheetcam will set the feedback correctly at the completion of a hole rule.

So lets use adaptive feed and motion.analog-out-01 instead
1. Connect motion .feed.hold to a motion.analog-out-01
2. Use M67 to set the analog pin to 1 at the start of your code (lets use motion.analog-out-01 for now) so M67 Q1 P1 P4 0.1
3. Enable adaptive feed at start of program with M50 P1
4. to set 60% of feed rate, your cutting rule should be M68 Q1 P0.6
5. to turn hole mode off (100% of feed rate again) M68 Q1 P1.0

Give it a go and report back. This has been worrying me a bit. You might be able to fully automate this as sheetcam has an onarc function that can calculate the arc radius. Maybe you could combine with with material thickness and make some decisions about how much to slow down by based on radius as a percentage of thickness.
Last edit: 05 Jun 2019 10:02 by rodw.

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

More
05 Jun 2019 10:31 #135923 by pl7i92
we did this on the plasma from 2012
with Mcode
#!/bin/bash
# thc enable off
halcmd setp thcud.enable False
exit 0

there is also a mcode for copletly rub the 24V from the THC module

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

More
05 Jun 2019 10:54 #135927 by rodw

pl7i92 wrote: we did this on the plasma from 2012
with Mcode

#!/bin/bash
# thc enable off
halcmd setp thcud.enable False
exit 0

there is also a mcode for completely rub the 24V from the THC module


But this is completely irrelevant to the topic here which is to do with plasmac, not THCUD and there is no need to turn the THC off as Plasmac will do that for us.

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

More
05 Jun 2019 15:42 - 05 Jun 2019 16:42 #135950 by Grotius
@Phill,

You do NOT need a cam program to use plasmac, I don't have one. All the samples are hand coded with the exception of the wrench which I think was originally done for my mill with dxftogcode.

Maybe you know i am trying to programming a dxf to gcode in c.
I started the c project with GTK and OpenGL and switched the project to QT c++ some time ago.

I just have made some progress to display some lines within QT. It's a stand alone program that can be called inside or outside of linuxcnc to generate parts from a dxf drawing.

My advise is to keep left a spare button in your PlasmaC Gmoccapy program wich has a image like CAM to startup a external cam program. Best way is to modernize the Gmocappy source code to call a external program using a screen button.
The python code for calling a external program via system takes about one line, so very easy to do.

@Rod,

In theory this should work just by changing the feed rate as the cornerlock feature of plasmac should kick in without the need to disable the THC from G code.

The sheetcam code widget's are really handy to use for small circles or shapes that need's presice accuracy. The standard is, that holes will result much nicer and will look nicer when cutting about 75% of contour cutting speed.
Me personally never used cornerlock or kerf crossing for plasma with all respect.
I think it's only usefull to use kerf crossing and cornerlock when switching a laser source into a plasma source on a german Trump laser. They are much more reactive.



For the future of Linuxcnc plasma we need a automated dxf layer based strategy, just like the code snippets provided in sheetcam.
Every layer has a option for speed or kerf or power etc.
And we need cam program's to provide a command line input option for linux system command. That will improve the power a lot.
Imagine that you don't have to start up a cam program. All system input's are done by linuxcnc. Output is direct ngc code.
This can be called a universal program standard without actually displaying the specific program, it run's in background. Only providing the code we want to achieve.

So manybe i have a different look at the future of cam related program's. This idea has evolved trough experience with linuxcnc.
The fear point of Cam provider's is the GPL2 licence. Draftsight 2019 update is very good, and non free for windows users, why?
It's only because Freecad become's more and more powerfull. Autodesk is afraid to loose the dominant position (microsoft position) trouhh very good open source cad program's. In the end everything will be open source. But we need to fear the GPL3 licences.
www.gnu.org/licenses/gpl-3.0.nl.html

en.wikipedia.org/wiki/Ubuntu
So we can distribute linuxcnc with Ubuntu wihout any problem or with LinuxMint, also a open source distribution.
Attachments:
Last edit: 05 Jun 2019 16:42 by Grotius.
The following user(s) said Thank You: phillc54

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

More
05 Jun 2019 18:04 #135967 by pl7i92
Freecad is realy far away from getting a good sketcher
so many things missing from Qcad libracad

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

Time to create page: 0.115 seconds
Powered by Kunena Forum