CNC Plasma ... using M209 and SheetCAM

This is the place to talk about and share things related to CNC plasma machines using UCCNC

CNC Plasma ... using M209 and SheetCAM

Postby Steve@MEM » Wed May 24, 2017 5:37 pm

Hello I'd welcome any pointers on the best approach ( or the options) for running the macro M209.
I'm on a learning curve on CNC in general ... so please bear with some inexperience here !

I'm about to switch from Mach 3 with Proma 150 THC and looking to implement anti-dive the best possible way.
Using M209, so that the THC function gets automatically enabled/disabled by the motion control code deep inside UCCNC.
This seems a good way to go.... it's what I plan to try. Advice would be welcomed on how to do this
For example ...
Is adapting the CAM program's post-processor the right way to ensures M209 {....} gets included in the header block of the G-code output ?
Is there another way in UCCNC to make sure M209 is run for each plasma profiling job ?
I also see 'code snippets' in SheetCAM which look like they could include M209 and pass it the minimum speed parameter in the {....} brackets.

Just about to dive into UCCNC and asking for any pointers so I swim in the right direction !

Thanks in advance, Steve
Posts: 1
Joined: Wed May 24, 2017 4:28 pm

Re: CNC Plasma ... using M209 and SheetCAM

Postby Robertspark » Wed Jun 07, 2017 8:31 pm

Sorry, I don't frequent the forum much at the moment

M209 & M210 are the THC anti-dive on and off (i.e. M209 inhibits downward motion, when the feedrate whilst cutting drops below the anti-dive feedrate (such as when cutting small circles (i.e. the torch will not be able to accelerate up to the feedrate before having the decelerate down (unless you have over-burn enabled [correctly]), or when the torch decelerates to change direction by say 90 degrees, as one axis must begin to decelerate whilst the other begines to accelerate, but at the midpoint of the motion, the combined feedrate would have dropped to around 70% of the straight line feedrate (or less) depending upon the corner error max setting).

Really M209 & M210 are actually nothing to do with THC and are an internal function within UCCNC that basically ignores the down signal from the THC when the feedrate drops below the defined setting.

I'd suggest if you are new to uccnc and using the Proma 150 (not the proma 150SD that is the stand alone one), forget about M209 for the start....

What you will need to do is enable and disable THC, this is done via the post processor within sheetcam (I think I posted a fair bit on this a while ago and even my postproccessor of the sheetcam forum).
Basically, if you want to use THC, enable and disable it with M205 (THC On) and M206 (THC off)

hence if your post processor header section had an M205, it will mean that you intend to use THC.

because you can control THC within uccnc much better than in Mach3 because of the way that there is no delay in triggering the THC on and off (we use to use M10 & M11 via other outputs in Mach3 as a fudge before) that is all you really need.....
Hence you can edit your post processor (or use snippets in sheetcam) to use a M206 before small circles of less than a certain size and corners, and M205 after the corners [you will have had to have enabled M205 earlier though...... ]

More advanced control (correct way to do it) is to use M205 at the start of your code, and use M209 with a low THC setting say 60-70% of the cutting feedrate, that way UCCNC will automatically inhibit the down motion when the torch first starts moving [see note below on M207] and slows down at corners and on small circles [depending upon you machines acceleration]
Then use M211 / M212 via snippet code before + after small circles and corners to turn off the downward motion when the torch is slowin down and speeding back up.
Then use M207 at the same time as you use M205 at the start of you code which will enable the THC delay whilst the arc is establishing at the start of the cut [ie it ignores THCUP and THC DN commands]

Word of note..... when THC is enabled, motion will not begin until the THCOK signal is recived from the THC. No THCOK, the torch will fire and that is it. the torch is fired by M3 and turned off via M5.

Uccnc has an added function that is built in..... if it losses the arc whist cutting (and THC is enabled!), the machine will disable M3 and stop and back up to the point that the arc was lost so that a restart can take place and cutting can continue from this point (there is a chance of a refire divot and maybe not a very clean cut at this point, a few of us have another way around this one, but it requires a secondary physical circuit for the torch fire signal).

Closing note..... the proma is not a very good THC (I still have one somewhere on the bench waiting for resale...) The reason being is it is not very fast at all. It also lacks a decent amount of settings which there is a partial fudge for .... to do with the pilot arc voltage setting. Also the voltage differential is quite large (i.e. it lacks accuracy).
For it's price its a starting point at very basic entry level. When you start chasing better cut quality and machine acceleration and cutting speed, plus storing settings within sheetcam for cutting voltages etc then it's time to change in my opinion.

If you want anything explaining a little more, just let me know and I'll try to help (I have a few days I'm likley to be about here).

goes across a gap / kerf or when the torch slows down and the voltage detected by the THC begins to rise, and the THC's automatic reaction is to dive to lower the voltage, M210 deactivates the THC anti-dive function.

In order to ue M209, you will also need M205

Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
UC400eth, UC300eth, UCCNC v1.2046, Neuron Lite.
UCCNC Macro Manual
Posts: 615
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England

Re: CNC Plasma ... using M209 and SheetCAM

Postby beefy » Thu Jun 08, 2017 6:59 am

Hi Steve,

I've always been a bit irritated by the non descriptive term "anti-dive". The reason is there are two very different types of anti-dive. One of them is part of a THC and the other is part of the motion controller (UCCNC).

I personally call them corner anti-dive (motion controller) and void anti-dive (THC).

Corner anti-dive is what UCCNC controls, and is related to feedrate. If you have it set at 90% then when the feedrate drops below 90% any up/down signals should be ignored.

Void anti-dive is very different indeed. The THC monitors for a sudden rise/level in voltage, such as what you get when the torch crosses over a void. The THC is programmed to "assume" this spike in voltage means the torch is crossing a kerf, or has even gone off the edge of the plate. It will cease sending the up/down signals while this voltage is excessively high, and only allow the up/down signals again once the voltage has came down again (indicating the torch is over solid metal again).

I use Sheetcam to insert the synchronous THC on/off commands M205/206, but not with the post processor. I use Sheetcams Path Rules, Action Points, and Code Snippets, to strategically place these macros wherever they may be needed for a particular cut. You don't normally change the post processor for each individual cut, but Path Rules, Action Points and Code Snippets are used on each individual cut file as required.

Say in a particular cut I wanted to slow down at a corner. I would use Path Rules to turn off THC and reduce feedrate just before the corner, and likewise the Path Rules would increase the feedrate and turn the THC back on coming out of the corner.

Learn all you can on Sheetcams Path Rules, Action Points, and Code Snippets and you'll really start to love Sheetcam.

Posts: 152
Joined: Mon Sep 05, 2016 10:34 am

Re: CNC Plasma ... using M209 and SheetCAM

Postby Robertspark » Thu Jun 08, 2017 2:42 pm

What he said ^^^^^ better explained than I....

Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
UC400eth, UC300eth, UCCNC v1.2046, Neuron Lite.
UCCNC Macro Manual
Posts: 615
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England

Return to CNC Plasma

Who is online

Users browsing this forum: No registered users and 1 guest