http://www.plasmaspider.com/viewtopic.php?f=3&t=5113
There is a feature used in this topic to wrap a 2d drawing around a tube with a given diameter using the 4th axis.
I can not reproduce this process in Sheetcam and I can not find the information in the manual.
How is Vmax549 (4th and 5th post in the topic) doing this?
I want to use this function for my tube notcher.
Hoping to find a explanation!
Jacala
The Netherlands.
Hi jacala,
this is my solution :
#1 Copy the pp in the attached zip file to the posts-directory of Sheetcam
#2 Suppose your tube or column has a diameter of 100 mm then the circumference has a length of 100 * PI where PI is 3.14159
#3 SC uses the Y-value of your drawing for calculations so draw in your favourite CAD software a rectangle of i.e. 50 mm in X and 314.159 in Y
#4 Add some text or other shapes like I did in my example, export this drawing in dxf format and import it to SC
#5 Select in SC from the menu Options → machine → post processor the pp from #1
#6 You need to add 2 variables to make this pp work :
one named Diameter
one named Angle
where angle is set to 0 if the surface of your tube isn’t conical
Both variables are case sensitive
#7 create an contour operation as usual and select the shapes you want to wrap
#8 start the pp by clicking on P in the top left corner and save the created file
This workes for me to create the attached files
Richard
Since I can upload only 3 attachments here is another screenshot with the variable Angle set to 10
Richard
First of all: What a great explanation and I owe you one!
I’ve installed the Post pr. and did exactly how you explaned.
I’ve got the processing figured out, at least I think I do.
I’m gonna fiddle with it because I’m hitting a little bump here and there. Still learning a lot.
Thanks and I’ll be back in a few hours with some questions 
MMM
for some reason I can export the file as g code but Mach 3 can’t work with it.
When exporting the same file with pp mach3 plasma it works great.
When exporting with Minimum G-code no arcs post processor (edited) there is an error in the beginning of the G code when viewing in Mach3
Bad character used: N0020 new function
N0020: new function
N0030: new function
N0040: new function
I’m searching for an answer but found none yet!
That is due to a bug in the post. I would guess it was put there for testing purposes. Go to Options->machine->post processor and click on the ‘edit post’ button. Look for:
function OnNewOperation()
In that function you will find:
post.Text(" new function\n ")
Delete that line, save the post and try it again.
Hello Les!
That worked a charm! Thanks.
Mach is showing the correct part now, y axis is moving, Z axis is moving so now only A axis, that one doesn’t do anything at the moment but also gives no reaction in mach3 when jogging A/4th axis stays 0.000
The G code gives the right data so there is a setting wrong in Mach, or at least I believe that is the problem.
The weird thing is that the ports and pins settings are correct and are enabled for Y, A and Z axis. Could have something to do that this pc runs only a demo version of Mach 3.
I’ll try it tomorrow on the real machine and come back with the results.
Were getting there. A bit more learning and searching to do Thanks.
Edit:
Reinstalled Mach 3 and problem solved! Looks great and cant wait to start cutting tube!
Hi jacala,
finally back from work. Read your reply but couldn’t answer from work.
Glad I could give you a kick in the right direction.
@LES
yes you were right.
I would guess it was put there for testing purposes
Just forgot to delete it. Thanks for your help
Richard
Hello!
Today I was tinkering again but while I changed nothing there is a weird fault in the G code.
For some reason the third line of G code is not functional and gives the A axis the command to keep rotating until it reaches a 20 digit number, so that could take a while .
You can see the attachement with the fault on line 3. I’ve tried a new different DXF but that changes nothing.
When I delete the line of G code it works just fine like yesterday. So, what could be causing this weird G code value?
Could you upload the drawing creating this code ?
Richard
In the attachment is the file. But it happens in all the files, also when I make a brand new file.
You can see the attachment, there are 2 files with both the problem.
It came up without changing anything to the settings so there is probably only 2 options: I’m doing something wrong or there is a bug.
No problems here with your files.
Did you set the variables correct ?
Looks to me as if your startpoint is pretty far away from the part itself.
How far away from X0 / Y0 is your drawing ? What are the values at the bottom of the SC window in the X and Y field ?
Richard
Mmm,
Nope, that seems fine by me but in the code editor you can see the weird value.
Reinstalling sheet cam could solve the glitch?
See attachment for more info.
Please upload the job file
Richard
In the attachment is the faulty code.
Thanks for helping me. Weird that something is changed in a day that gives this error.
Good luck checking it out!
Looks like the PP doesn’t like calculations with negative numbers.
Please remove in the PP in the following functions the red bold characters .
This will result in positive A-values and you might mirror the rotational direction of the A-axis in Mach3
Hope this helps
Richard
function OnRapid()
radius = Diameter / 2
post.Text (" G00")
post.ModalNumber (" X", endX * scale, “0.000”)
post.ModalNumber (" A", endY * 180 / 3.14159 / radius -1,“0.000”)
post.ModalNumber (" Z", (endZ + math.tan(Angle/1803.14159) * endX + toolOffset) * scale, “0.000”)
post.Eol()
end
function OnMove()
radius = Diameter / 2
post.Text (" G01")
post.ModalNumber (" X", endX * scale, “0.000”)
post.ModalNumber (" A", endY * 180 / 3.14159 / radius -1,“0.000”)
post.ModalNumber (" Z", (endZ + math.tan(Angle/1803.14159) * endX + toolOffset) * scale, “0.000”)
post.ModalNumber (" F", feedRate * scale, “0.###”)
post.ModalNumber (" S", spindleSpeed, “0.##”)
post.Eol()
end
That did the trick.
Thanks! Where would you like your statue to be build?
Hi Guus,
please build my statue where all my others where built :
http://i2.cdn.turner.com/cnn/dam/assets/130102082353-easter-island-moai-horizontal-gallery.jpg
Thanks
Richard 
Hello!
you’re a great man when you got your own easter island. Must be difficult to stay normal and help full to us simple humans.
I’m at the next stage and searching/testing to solve it:
At the moment M03 (plasma on) and M05 (plasma off) are not in the G code of the Post.
I’ve been searching in the mach3 plasma Post because M03/M05 is present and working there but to no result yet. I tried to export the lines that I thought send the M03 and M05 code but that did not work. It should be quite simple so I’m gonna try and find it.
After digging in the Mach 3 Plasma post I’ve found a line that helps a bit but surely is not good enough yet.
I’ve managed to include the M05 and M03 commands into the G code, the problem now it that it is repeated every single command.
I took this line out of the Mach 3 plasma post
post.Text (“\n M03\n”)
And pasted in a copy of the working rotary post like this:
function OnRapid()
radius = Diameter / 2
post.Text (" G00")
post.Text (“\n M05\n”)
post.ModalNumber (" X", endX * scale, “0.000”)
post.ModalNumber (" A", endY * 180 / 3.14159 / radius ,“0.000”)
post.ModalNumber (" Z", (endZ + math.tan(Angle/180*3.14159) * endX + toolOffset) * scale, “0.000”)
post.Eol()
end
function OnMove()
radius = Diameter / 2
post.Text (" G01")
post.Text (“\n M03\n”)
post.ModalNumber (" X", endX * scale, “0.000”)
post.ModalNumber (" A", endY * 180 / 3.14159 / radius ,“0.000”)
post.ModalNumber (" Z", (endZ + math.tan(Angle/180*3.14159) * endX + toolOffset) * scale, “0.000”)
post.ModalNumber (" F", feedRate * scale, “0.###”)
post.ModalNumber (" S", spindleSpeed, “0.##”)
post.Eol()
end
Ofcourse it was just a try with the result of giving th M03 or M05 command every line (as you can see in the attachment). The mach 3 plasma post does not have this so this is a small step but not in the right direction so fat What am I doing wrong?