Centre spotting with Hypertherm Powermax45 XP

More
09 Dec 2020 08:14 #191479 by Zultan
After recently updating to the newest version of Plasmac I have been playing with the centre spotting feature. My machine is using mode 2 (proma external thc) and a regular parallel port breakout board combo (no fancy Mesa stuff here). I am getting strange results where the torch will only spot every second hole so #1,3,5 while skipping #2,4,6. Having read other threads where similar behavior is reported I added a delay and found that a delay of ~20s will allow the torch to fire every time. Interestingly 20s is also the amount of time that 45XP uses for postflow air.
When i played with manually pulsing the torch I see that the first pulse fires and the runs post flow, the next pulse causes the post flow to stop and the third pulse once again fires and turns on post flow so his seems to be a feature of the machine. Additionally the machine manual states on p53 "For the machine torch, run a START/STOP command from the CNC to cause the torch to emit the puffs of air. On the next start signal, the torch will fire an arc."
I was wondering if there is a way to send a torch fire signal from gcode so that I can modify a post processor that pulses the torch before M3. I think a gcode solution would be preferable since then it will not effect people who don't have this problem.

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

More
09 Dec 2020 10:53 #191485 by tommylight
An easy solution would be to use the "search and replace" or CTRL+H feature of the text editor to add a short pause and another M3 after every existing M3.

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

More
09 Dec 2020 10:58 - 09 Dec 2020 10:59 #191486 by snowgoer540

An easy solution would be to use the "search and replace" or CTRL+H feature of the text editor to add a short pause and another M3 after every existing M3.


I'm not sure that will work because it doesn't actually fire the torch until it finds the material. It would need to probe and find the material first. Sounds like he needs 2 torch pulses (really ON, OFF (probably with some small time delay in between), then ON (with the appropriate timer)) after the material height is found.

But I am still on coffee #1, so forgive me if I'm way off base :)
Last edit: 09 Dec 2020 10:59 by snowgoer540.
The following user(s) said Thank You: tommylight

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

More
09 Dec 2020 11:18 #191487 by tommylight


But I am still on coffee #1, so forgive me if I'm way off base :)

Same here. :)
And you are right that would cause two probes for each spot. Not deal breaking, but time consuming.

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

More
09 Dec 2020 11:56 - 10 Dec 2020 00:17 #191490 by phillc54
I think you could connect the plasmac:spotting-start signal to the input of a one shot and connect the oneshot output to a or2. Disconnect the torch Hal pin from the plasmac:torch-on signal and connect it to the or2 output then connect the plasmac:torch-on signal to the other or2 input. Set the pulse time on the oneshot.
This way it will automatically pulse the torch whenever it gets a spotting start signal.

EDIT: It works well in a sim, the only proviso is that the pulse needs to be shorter than the time it takes to probe and move to pierce height.
Last edit: 10 Dec 2020 00:17 by phillc54.
The following user(s) said Thank You: tommylight

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

More
08 Apr 2021 21:04 #205364 by AgentWD40
If I may tag along on an old thread...

I'm having trouble getting this feature to work. I used the code provided in the plasmac user guide. linuxcnc.org/docs/2.8/html/plasma/plasma...-guide.html#spotting

Multi-tool is enabled in the hal file.

It will run through the code but simply doesn't fire the torch.

I'm also using a hypertherm powermax 45xp.

Can someone post sample gcode that will simply mark a centre spot where ever the torch is currently jogged to?

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

More
09 Apr 2021 00:23 #205388 by snowgoer540
The sample code in the docs should work...

I am curious what is your spotting "time on" set to? It could be too fast for the hypertherm to recognize...
The following user(s) said Thank You: AgentWD40

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

More
09 Apr 2021 01:07 #205390 by AgentWD40
I didn't even try playing with the spot time setting... I'm a knuckle head. I'll give it a shot tomorrow.
The following user(s) said Thank You: snowgoer540

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

More
09 Apr 2021 07:32 - 09 Apr 2021 07:32 #205400 by rodw
Normally you will use sheetcam with a special tool called you define Centre Spot (or Center Spot for the Americans) and have the holes laid out in the file at normal size. Then You move all holes onto a new layer. Run a drill operation in Sheetcam on the holes layer with then centre spot tool, then create a new jet (plasma) operation to cut the outlines. There are also settings in sheetcam that will spot holes < a defined diameter.
Last edit: 09 Apr 2021 07:32 by rodw.
The following user(s) said Thank You: AgentWD40

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

More
09 Apr 2021 14:45 - 09 Apr 2021 15:03 #205436 by AgentWD40
Time setting of 200 and dialing the amperage down to 10 did the trick!

I'm not too familiar with sheetcam's pp language.

I've found I need to add about a 10 second dwell between each spot. What would be the code exactly to modify the pp?

I've found this in the pp. Would this change suffice?
function OnPenUp()
    post.Text ('\n M5 $', spindleNum, '(', cutName, ' stop)\n')
    if string.match (toolName, 'Air Scribe') then
        post.Text (' G4 P1 (pause for scribe retract)\n')


-- BEGIN MY CHANGES
    elseif cutType == 'Spotting' then
        post.Text (' G4 P10 (pause between spots)\n')
-- END MY CHANGES


    end
        post.Text (';end operation #', cut, ', ',string.lower(cutType), '\n')
    cut = cut + 1
end

(edit)
I made the proposed change and it seems to be working as expected.

Now what I would like to know if there is a way to get the pp to pause the program before and after a set of drilling operations and display a message box in linuxcnc to tell the user to manually adjust the amperage on the plasma cutter??
Last edit: 09 Apr 2021 15:03 by AgentWD40.

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

Moderators: phillc54
Time to create page: 0.107 seconds
Powered by Kunena Forum