Z axis speed setting for THC.

Having problems with or questions about SheetCam? Post them here.
Post Reply
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Z axis speed setting for THC.

Post by Cncburn »

Is there a way to adjust my Z axis speed automatically when my THC is on? I have modified my post and added: M667 F20 as an example. But I have to do that for each material (tool), because the thickness / travel speed changes. Can I put in a line of code that would reference the tool /speed used and adjust the THC Z speed as a percentage of the tool speed? Example 1/4” steel cuts at 48 ipm, so my THC line would be M667 F (refTool *.5), The exact speed correction is still to be determined.
I am using a capacitive THC with a Masso controller and DMM servo drives. Thank you,
robertspark
Posts: 257
Joined: Thu Feb 26, 2015 12:11 am

Re: Z axis speed setting for THC.

Post by robertspark »

you can add it to the post processor file so that an extra text box is added to the tool table.

I would suggest you have a look at the candcnc post processors installed as default. at the start of the code befor oninit() there is a section that defines additional thc voltages that the candcnc postprocessor requires and passes to their THC as part of the code.

within the post processor documentation it explains the defined variables and adding additional custom boxes to the tools or process that you can then automatically pass to the controller via gcode sequence
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

Thank you for the advice. I will look into it.
robertspark
Posts: 257
Joined: Thu Feb 26, 2015 12:11 am

Re: Z axis speed setting for THC.

Post by robertspark »

Now I am in front of a laptop and not a phone I can give you a bit more information....

It you open up the default installed CandCNCPlasmaLLCNC-rev16.scpost post processor you'll see that it has

Code: Select all

post.DefineCustomToolParam("PlasmaTool", "Preset volts", "presetVolts", sc.unit0DECPLACE, 49, 0, 200)

The "post.DefineCustomToolParam" function allows you to define those additional test boxes that could be added to any of the tools.

In this case
DefineCustomToolParam(toolClass,caption,varName,units,default,min,max)
Adds an extra parameter to a tool definition.
toolClass is the tool class name. See the toolClass variable for a description of tool classes
default is the default value. Note that values are always in METRIC for linear units, RADIANS for angular units and a decimal fraction for percentage e.g 0.1 = 10%
The rest of the syntax is as DefineVariable

DefineVariable(varName,units,min,max)
Define a variable name for use in the ‘set variable’ dialog.
varName = variable name
units. One of the following: sc.unitTEXT, sc.unitLINEAR, sc.unitANGULAR, sc.unitFEED, sc.unitRPM, sc.unitTIME, sc.unitPERCENT, sc.unitPITCH,
sc.unit0DECPLACE, sc.unit1DECPLACE, sc.unit2DECPLACE, ,sc.unit3DECPLACE, sc.unit4DECPLACE note the unitxDECPLACE units display
a number without units with a precision of the given number of decimal places
min minimum value (ignored for text)
max maximum value (ignored for text)
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

I'll give it a try. Thank you
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

Ok, I looked into your solution a little last night. If I understand correctly, this will give me an additional text box for each tool. I would then enter a custom Z speed for each tool in the new text box. When the tool is used, and the THC is called, it would run the Z axis at the speed posted for that tool. Is that correct? Thank you
User avatar
Les Newell
Site Admin
Posts: 3661
Joined: Thu May 11, 2006 8:12 pm

Re: Z axis speed setting for THC.

Post by Les Newell »

in the function OnToolChange() add this code:

Code: Select all

   post.Text(" M667 F")
   post.Number(feedRate * 0.5 * scale, "0.##")
   post.Eol()
That will output the M667 feed rate as 50% of the cutting feed rate. You can obviously change the percentage to suit.
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

Thank you so much. That is exactly what I was looking for.
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

I did not have the function onToolchange() in my post. I did have a Function ThcOn(). So I put the command there. It appears to be working. Thank you
User avatar
djreiswig
Posts: 471
Joined: Sat Feb 20, 2016 4:47 am
Location: SE Nebraska

Re: Z axis speed setting for THC.

Post by djreiswig »

You can add the function of it isn't there.
User avatar
Les Newell
Site Admin
Posts: 3661
Joined: Thu May 11, 2006 8:12 pm

Re: Z axis speed setting for THC.

Post by Les Newell »

Putting it in THCon should work. You can create your own OnToolChange()

Code: Select all

function OnToolChange()
   post.Text(" M667 F")
   post.Number(feedRate * 0.5 * scale, "0.##")
   post.Eol()
end
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

Thanks again Les. It seems to be working in the THC area. Somehow, I also managed to install a post variable for THC ON & 15%. I think it is also having some affect as well. I just have not had time to play with it to see all of the results. Looking forward to some quality time in the garage :lol: Eventually, I will build separate Posts with each option to see which works the best. I do appreciate the help, and I love the Sheetcam software.
MetalheadF13
Posts: 8
Joined: Tue Jun 04, 2019 10:58 pm

Re: Z axis speed setting for THC.

Post by MetalheadF13 »

Hi is it possible to achieve setting the THC feed with path rules? I've just learned how to utilize path rules and its awesome just like the sheetcam software itself wish I found it sooner.
sheetcam/planet-cnc mk3 controller/ planet-cnc 10.30 software/powermax 45xp ohmic/ proma compact THC/ DIY plasma table , 0lll0
Cncburn
Posts: 18
Joined: Wed Apr 17, 2019 6:38 pm
Location: Land O Lakes, Fl. USA

Re: Z axis speed setting for THC.

Post by Cncburn »

Just my limited experience talking here. If I had to just change the THC speed to just one setting, I would modify the post on the line that calls the THC on: right after M667 add F and the speed.

function ThcOn()
if(thcstate ==0) then
thcstate = 1
post.Text(" M667 F40 (---THC on---)\n");
return
end
if(thcstate == 2) then
thcstate = 0
end
end
Post Reply