CandCNC thc and rotary axis

Hi All

Having some issues getting my rotary axis setup correctly, I have a CandCNC BladeRunner Dragon Cut 620-5 control system, if i utilise the post HTHCII-DTHCIVRotaryPipeFit-setacis_REV3 there are a few issues:

  1. as soon as I load the gcode it pops up that the pipe od has been set for 1 inch (my machine is all setup in metric) and also the file was draw and setup in sheetcam for 76mm tube.

2)It then automatically sets the steps and speed of the axis (i assume to accommodate 1 inch tube not the 76)

  1. if i do dry run the file it is moving along my Y axis instead of X axis as the length of the tube.

If i use the normal mach3 rotary post then there is no auto setting of the steps etc so it keeps what i have put and motion appears mostly correct with some strange slowdown and jumpy movement on the sides of circles otherwise it mostly runs correctly. problem being it then doesn’t include any of the THC commands or control.

On a side note if i try the screen set for rotary that came with the candcnc system it has a “test 1 revolution button” along with some settings etc, if i set 2000 steps with a 1:3 gear reduction (which is what i have) and click test it does spin 1 revolution (50% at full speed and 50 at a reduced speed) but if i look at the dro it only reads 36 (not 360) if i then change it to 200 steps (as if no micro stepping) then the test button doesn’t spin it a full revolution yet typing G0 B360 does spin 1 revolution.


Ok I received some feedback from CandCNC, aparently their post does not work with metric so im kinda left out in the cold…

So I have reverted back to my standard post,which includes all my thc etc features, that I have been using (for flat sheet) and edited it to include the rotaryAxis and unitsPerRev in the settings as well as adding post.ModalNumber (" " … rotaryAxis, endA, “0.0000”) in the OnRapid, OnMove and OnArc functions.
I also added the two lines :
package.path = sc.Globals:Get().thisDir … “/plugins/RotaryPlasma/?.lua”

all as per your vid Les, It did make some headway butnow my issues are as follows:

Right at the start of the gcode file (line 7) i get a Z30 move, machine pauses at this point aswell, if i click run again it then carries on but immediately after a torch fire command i am getting an M11 command that is then lifting the torch head ±30mm away from the part (see line 35 as eg)

I have now managed to get the rotary axis elements included into my normal post, so i now have my touch-off and thc all functioning, I also dont need to change post’s when i am working on flat sheet vs pipe.

I believe this adds some to the calcs and processor load but from analysing a few gcode files pre and post change I dont really see any differences, in fact after the code is parsed through the lua script its a bit cleaner, I had to add some basic rules for the thc but in essence it is working… sort of…

I still have the issue where after the pierce the torch is lifting to 39.5mm I now see this is the pipes radius, so what I think is happening is the torch is touching off on the pipe, setting 0 but that is being seen as the centre line of the pipe. so it then lifts to the radius…

Les is there any way i can stop it from doing that?

When cutting pipe it needs to use the center line of the pipe as Z0. If you have added your own touch-off code you need to take this into account. Take a look at function Reference() inthe RotaryPlasma Mach3 post to see how this is done. The code works for flat sheet as well. In that case Z0 is the top of the work.

Excellent thank you Les!!

I also had to add the query and matz to the pendown function for pierce height settings, but all working now, on both tube and flat sheet :slight_smile:

I now have a question on the rotational movement when it gets to a straight line, it is very “jumpy” it is breaking the line into 0.7626mm lengths in the gcode, if it is an arc the rotational motion seems to be smooth, but on straight lines it goes code heavy and jumpy, this becomes apparent on two sides of circles as well, the same happens with the standard mach 3 rotary post so I am assuming its some setting I have missed somewhere??

What version of SheetCam are you using?

Development V 6.1.38

I am running a Hypertherm with the rs485 connection

You having said that made me wonder about the normal version, I tested and the motion is stable in normal sheetcam, I also imported my toolset and it seemed like all the additional variables (air pressure, amps etc) seems to have come in now.

Am I able to use all the dcc variables now in the normal version of sheetcam (was pretty much the only reason i had been using development from original candcnc instructions)

On some further investigation the outputted g-code is still giving 1 error, before every touch-off it is including a line to go to pierce height, see attached image. i set a test tool with a random pierce height to check this (12.3).

The only reference i have to pierceheight is in my function OnPenDown() as per below:
post.ModalText (" G00 “)
post.Text(” Z")
post.Number ((matZ + pierceHeight) * scale, “0.0000”)

this random line does not seem to follow this as it does not include the G00