SheetCam Plasma Post Processor, with working THC codes! (FIXED) "Includes Scribe"

Ross

Ross
I have noticed a few members having plasma post processor problems.

The Masso one that I edited has the THC "ON OFF" values added to it and is working correctly.

It allows the THC to turn on and off when needed at the (start of cutting), (during cutting) plus at the (end of the cut).

Allowing the Z axis to go to safe rapids height between cuts.

In SheetCam you will have to edit the post processor to suit your Z axis travel limits of your machine.

I have also add to the M667 F150 this changes the feed rate of the Z axis while the THC is active, (THIS IS A HAPPY SPEED FOR THE THC) You can change this to your own likening, This is set in millimetres cause I use metric (not sure about imperial though)

I have posted this before on the forum and it includes photos as well.

Here is the postscript again.

"Photo Attached, shows were to edit your Z travel limit in SheetCam to suit your Machine"

from Ross.

PS, Give a thumbs up if you down load my Post Processor so i have an idea how many of you use it, thanks!
 

Attachments

  • MASSO-Plasma-with-THC-and-Scribe-Ross-Woolley-G04-in-milliseconds.scpost
    9.4 KB · Views: 69
  • Z-Distance.png
    Z-Distance.png
    192.6 KB · Views: 44

Ross

Ross
Just save to computer, as SCPOST file.

In Sheetcam: Options/ machine/ Post Processor/ Import Post.
 

justingro

Justingro
hi Guys . Ross.

thanks for that but i am using fusion 360 and not sheetcam i have posted my post processor here i have no speed component behind my m667 code but in my post proprieties i have a thc min speed in upm but doesn't seem to do any thing will post a clip once happy .But z axis is going up and down with the sheet just got to get the right voltage setting to get the right cut height .But it does want to play catch up on the downward slop increasing gap between touch and plate by 4mm slowing every thing down helps
 

Attachments

  • masso-plasma-60-hole-reduction-probe.zip
    6 KB · Views: 30

svenn-m

Svenn-m
Quote from Ross on June 17, 2019, 1:20 pm

I have noticed a few members having plasma post processor problems.

The Masso one that I edited has the THC "ON OFF" values added to it and is working correctly.

It allows the THC to turn on and off when needed at the (start of cutting), (during cutting) plus at the (end of the cut).

Allowing the Z axis to go to safe rapids height between cuts.

In SheetCam you will have to edit the post processor to suit your Z axis travel limits of your machine.

I have also add to the M667 F150 this changes the feed rate of the Z axis while the THC is active, (THIS IS A HAPPY SPEED FOR THE THC) You can change this to your own likening, This is set in millimeters cause I use metric (not sure about imperial though)

I have posted this before on the forum and it includes photos as well.

Here is the postscript again.

from Ross.

Ps, Give a thumbs up if you down load my Post Processor so i have an idea how many of you use it, thanks!

Hi Ross

When I use your Post Processor, I get a Z soft limit error. Where do I change this in the Post Processor?
Svenn
 

Ross

Ross
Hi Svenn, Change your Z distance in the Post Processor. Edit and save.

Photo shows where to do it.

From Ross.
 

Attachments

  • Z-Distance.png
    Z-Distance.png
    192.6 KB · Views: 32

Ross

Ross
By changing the value in SheetCam were shown in photo below, it will slow down and turn off the THC for the size that you make.

SlowPercent is the actual percentage you want to slow down by. 0.4 is cut speed -60% of your set speed.

Hope this helps.

Ross.
 

Attachments

  • Radius-hole-size.png
    Radius-hole-size.png
    197.4 KB · Views: 34

Ross

Ross
It will slow and turn off THC on all sharp corners.

If you make a square of any size and produce a G-code, then open it in notepad you can see the THC on/off as-well as the slow down in the feed rate.

From Ross.
 

fablab

Fablab
Ross,

I would just like to thank you very much for your post processor!! It is working just awesome for me.
I just made a few minor tweaks for my homebuilt machine & so far it is almost perfect. The only thing I would like to change (its not a big deal) and I haven't figured out how to do, is eliminate the initial Z probe cycle, with my setup I don't need it. It doesn't hurt anything, I just don't need it for my configuration, any pointers on how to remove it & not break anything else would be greatly appreciated.

I have attached a copy of my running post if that helps.



Again Thank You!!
 

Attachments

  • FabLabPost.scpost
    9.3 KB · Views: 25

Ross

Ross
Hi Fablab,

The probe is needed,

It's function is to obtain a zero reference. Other wise it will have no idea were the job is!

Probe function is done for plasma, then sets a reference of zero then will go to piece height.

Scribe is the above mentioned with the added offsets added for the scribe.

Hope this helps, Ross. PS: I notice you added the park G30 in the script, "Nice" post.Text (" M05 G30 M30 (---End of program---)\n")
 

Ross

Ross
"Changing the Z height on finish"

This is not necessary. But on finish, if you would like to raise the Z higher on the finish.
Change the value from 0 to the height you like.
(Caution) My Z safe travel is set at 45mm, by adding the value of 55mm means
End Z is going to be 100mm from job.
Note: if to high you will get a Z limit alarm on the Masso.

From Ross.
 

Attachments

  • Safe-Z-on-finish.jpg
    Safe-Z-on-finish.jpg
    223.1 KB · Views: 30

jcoldon

jcoldon
Ross have you used masso with a M01 pause command then restart the the plasma . this way one can do plate marking with lower amp setting do a m01 stop raise up amps then start cutting

sheet cam does all this . and not in post processor is a code snipet add in
 

jcoldon

jcoldon
i going to check this post out this looks like the one from command cnc mach 3 it has a problem cutting open lines at full feed rate i have sheet cam looking in to mine for uccnc

i going to see if my masso does the same with this post on the file i have .
 

fablab

Fablab
Quote from Ross on March 21, 2021, 1:41 pm

Hi Fablab,

The probe is needed,

It's function is to obtain a zero reference. Other wise it will have no idea were the job is!

Probe function is done for plasma, then sets a reference of zero then will go to piece height.

Scribe is the above mentioned with the added offsets added for the scribe.

Hope this helps, Ross. PS: I notice you added the park G30 in the script, "Nice" post.Text (" M05 G30 M30 (---End of program---)\n")

I completely understand what your saying & your right when I am cutting, however when scribing I don't need to take a Z reference. In my case the scribe & the torch don't share a screw.

The torch is mechanically (Z Axis) driven and the scribe is purely pneumatic (the height is controlled with an air cylinder) via. M7 & M9.

Does that make sense?

Please let me be clear this is not a complaint nor a criticism as I said before your post works great & I am very happy with it, I guess I just always have to tinker around with things :)
 

Ross

Ross
Hey fellers, I,m just fumbling though this myself and only been in this for two years! Like i can't even get square edge cuts yet!

Jcoldon, Haven't thought about the M01 trick yet, I'm a long way of from thinking about that. but i will add a video from JD Squared showing how their plasma behaves for motion!

Just racking my brain on how to get a router fitted to my Z axis at the moment, just going though all the options i could try.

Hi Fablab, Didn't realize the scribe was separate to the Z axis, so this is just a stab in the dark for me, but i think it has to changed here in the script.

--Scriber X,Y,Z offsets in MILLIMETRES. Do not use inches here even if you want inch code
--Use the special code 'nil' on the Z axis to disable it.
--In that case no Z values will be output at all while scribing.
--e.g scriberZ = nil
scriberX = 61.355

scriberY = 28.246
scriberZ = nil

--scriber axis. Leave this as nil if the scriber is fixed to the same axis as the torch
--scriberAxis = "A"
scriberAxis = nil


--If this value is true then use G28 (home) for Z reference
--set it to false for G38.2 probe
refHome = false


OK after looking at the script maybe just change the false to "true or G28"

I have no idea if this is the fix or not but it is the only thing i can see.

Good luck!

Well here is the video, if Masso can get these movements, especially from the Scribe were on a winner.

From Ross.

 
Top