Looking for some help dialing in a Proma SD on a new machine

Cut quality issues can be discussed here, most common issues have been discussed here and should help you.
Post Reply
xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Wed Jul 29, 2020 11:07 pm

Thank you.

I have UCCNC mostly configured and the controller bench tested. I should have it on the machine in the next day or so.

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Thu Jul 30, 2020 11:38 am

I have the controller configured and ready to mount on the machine. I may need to change some input wiring for the probe depending on the answers to below.

@robertspark - I remember reading a post from you on UCCNC and using 2 probes and you had it setup that if the ohmic failed it would default to the floating and apply the correct offset. For the life of me I am unable to find that post now when I search. In order to make this work do you use a separate input for the ohmic and the floating (ie not shared input)? I do have the ohmic on a relay and will need to determine how to have the ohmic off during cutting (sheetcam post processor or UCCNC). Which post processor are you using for UCCNC with your setup?

Thanks

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 1122
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Looking for some help dialing in a Proma SD on a new machine

Post by robertspark » Thu Jul 30, 2020 5:03 pm

xnaron wrote:
Thu Jul 30, 2020 11:38 am
I remember reading a post from you on UCCNC and using 2 probes and you had it setup that if the ohmic failed it would default to the floating and apply the correct offset. For the life of me I am unable to find that post now when I search. In order to make this work do you use a separate input for the ohmic and the floating (ie not shared input)? I do have the ohmic on a relay and will need to determine how to have the ohmic off during cutting (sheetcam post processor or UCCNC).
I wrote a macro which checks an input pin, but it needs a relay too and an output pin.

here is the macro.
http://www.forum.cncdrive.com/viewtopic ... 19661#p890


there are other ways to do this too.... when I wrote this macro UCCNC did not have the ability to have two probe inputs defined now it does.
Unfortunately, uccnc does not (appear) to have the ability to tell you which probe input is triggered..... but via macro you could check which input is active and then apply the correct offset.... what you cannot do when you use two probe inputs is ignore one if one is already triggered..... which is what I did with my macro and simple relay output interface. As sometimes I have had crud collect on the inside of the shield which has given me a false trip signal.... my macro has the ability to just ignore that and continue as normal using the floating head.

whatever works for you is best for you.


The procedure is as follows:

Macro M1031 gets called by sheetcam.
The macro checks if the probe input is active.
  • If it is active then it will stop and flag a message to the status message box and wait for a restart once you've checked things out (you could call a "park macro" so you access the torch easier and then send it back to your last cut position after you've checked things out but this would be additional macros and altering the M200-2 macros with the park positions or adding your own macros).
If the probe input is NOT active, then it will close the relay and retest the probe input.
  • If it is active then it will open the relay, throw a status message to the status message box and continue but NOT use the ohmic probe input, it will just use the floating head input

    It will perform now perform a G31 touchoff route and apply the floating head switch offset and hand back to UCCNC to continue the gcode sequence.
  • if the probe input remains unactive when it tests it for the second time above, then it will perform a G31 touchoff and when motion stops it will check which input was triggered by opening the relay and checking the probe input ..... if it is now NOT active it knows that the touchoff was via the ohmic probe input. If it is still active it knows that the touchoff was via the floating head and applies the correct offset and hands back to uccnc to continue the gcode.

note: I use the word "active" as it could be high or low as an active state via the probe settings checkbox.
xnaron wrote:
Thu Jul 30, 2020 11:38 am
Which post processor are you using for UCCNC with your setup?
I have written my own largely, but they were based upon the Mach3 generic one (I had some problems with a sheetcam post processor breaking mill tools when I first started out.... it's never been fixed (I just checked)
https://forum.sheetcam.com/viewtopic.ph ... nge#p22460

Doveryáy, no proveryáy https://en.wikipedia.org/wiki/Trust,_but_verify

if you don't understand it you cannot verify it.... hence I learned to write my own / check them before using them and clean up code I don't like or think is useful to me (YMMV)


As I have just posted in another thread most motion gcode and generic M-codes in Mach3, Mach4, UCCNC and Linuxcnc are the same so you can use one of those and just modify them to your needs.

If you have a hypertherm with a machine interface (not CPC, the RS485 (rectangular vertical pinout on the rear)) you can control the current from within UCCNC using the RS485 / modbus plugin and some modifications to your screenset + macros and macroloops

my touchoff is done within a MACRO within UCCNC and not via sheetcam. Sheetcam just calls the macro within the OnPenDown() method.

Code: Select all

   post.Text ("\n M1031\n")
   post.Text ("\n M03\n")
   if (pierceDelay > 0.001) then
      post.Text (" G04 P")
      post.Number (pierceDelay,"0.###")
      post.Eol()
   end
end
Oh check your pierce delay default setting in UCCNC is for the delay in miliseconds and not seconds, you can change it on the Settings >> General Setup tab



On sheetcam.... I also modify all of my post processors with the following, so that the operation appears in the right location (for me), but its just cosmetic

Code: Select all

function OnNewOperation()
   OperationFlag = 1
   --post.Text (" (Operation: ", operationName, ")\n")
end

Code: Select all

function OnRapid()
   if(OperationFlag == 1) then
      post.Text (" (Operation: ", operationName, ")\n")
      OperationFlag = 0
   end
and at the start of the file (define the new variable)

Code: Select all

OperationFlag = 0

I think you asked somewhere what version of UCCNC I use: I use the development version and only a few times have I ever found an issue as they are beta versions. If its all about the money then use the stable release..... but all the new stuff that comes out is in the development releases which are available here and you can read what has changed / been added as they are released. COVID19 has slowed cncDrive down as I think Hungary has been hit hard with lockdowns etc
http://www.forum.cncdrive.com/viewtopic ... 240#p18850
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Thu Jul 30, 2020 9:34 pm

Thanks. I will review as soon as I figure out why I can't get the torch to stay on. I click the torch on in the gui and the torch fires for a second and then it shuts off due toestop or limit. It alternates between estop and limit each time I try it. I've been checking my ports and pins and I don't see any conflict I don't know what could cause this. I have disconnected the 52 one from the controller as well as the ark okay. this is probably some safety feature I'm not aware of but I don't know. I'm trying to work my way through it now logically I'm really hoping it's not some type of interference issue from the PowerMax. I didn't have any at all with a cheap crossfire controller. Fingers crossed I'm doing something wrong and it's just some type of config issue in uccnc

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Thu Jul 30, 2020 9:38 pm

Crap. I disconnected the limits and estop plugs from the back and the torch will stay on. So it appears this is some type of interference issue :(. I guess I was just lucky with the crossfire all the wiring was pretty much the same as what I'm running here. Except for all the wiring in the new controller of course. The limits and I believe the East off or wired normally open which of course is in good for interference. I can't switch them to normally closed without redoing all the wiring to them.

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Thu Jul 30, 2020 9:51 pm

It was easy to wire the estop switch for normally closed and I left the limits unplugged and the torch stays on. I can rewire the limits later. My floating probe is wired normally open as well so I'm assuming that's going to cause issues and I'll need to change that too. I knew I shouldn't have wired them normally open I just copied what somebody else had done with the same machine because it worked for him. I should have went with my gut and wear them normally closed.

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Thu Jul 30, 2020 10:22 pm

I think I have the problem fixed. I put a 20ms debounce on the inputs and it seems to work now.

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 11:49 am

robertspark wrote:
Sat Jul 18, 2020 11:46 am

I was thinking about maybe having a go at a uccnc plugin thc this afternoon (I don't have need for one but I did wonder about bringing the cost of thc down via a simple plugin comparator board for the axbbe or uc400eth or uc300eth).... the cost below that of the minithc and the price avhc as the display and twiddly knobs are not required

I have used a lot of breakout boards in the past .... any CNC lpt board will do (I have a ud1 from cncroom and a uc1 too
The axbb-e has an analog input for 0 to 5 volts. I wonder if it could be used to monitor the voltage by a UCCNC plugin?

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 1:09 pm

robertspark wrote:
Thu Jul 30, 2020 5:03 pm


The procedure is as follows:

Macro M1031 gets called by sheetcam.
The macro checks if the probe input is active.
  • If it is active then it will stop and flag a message to the status message box and wait for a restart once you've checked things out (you could call a "park macro" so you access the torch easier and then send it back to your last cut position after you've checked things out but this would be additional macros and altering the M200-2 macros with the park positions or adding your own macros).
If the probe input is NOT active, then it will close the relay and retest the probe input.
  • If it is active then it will open the relay, throw a status message to the status message box and continue but NOT use the ohmic probe input, it will just use the floating head input

    It will perform now perform a G31 touchoff route and apply the floating head switch offset and hand back to UCCNC to continue the gcode sequence.
  • if the probe input remains unactive when it tests it for the second time above, then it will perform a G31 touchoff and when motion stops it will check which input was triggered by opening the relay and checking the probe input ..... if it is now NOT active it knows that the touchoff was via the ohmic probe input. If it is still active it knows that the touchoff was via the floating head and applies the correct offset and hands back to uccnc to continue the gcode.
Ok I actually had it wired like this. Both the ohmic and floating connected to a single input. The ohmic was connected to a relay and an output so I could switch it on and off (in parallel with the floating). It is easy for me to move it back to the single input and implement your macro. I will do this and test.

Now specific to my Proma SD. I am going to use this until I can get a price thc from xtremesystems. I have added 2 relays though to provide further control.
- Z inhibit. Relay connects to an output on the controller and allows the Z step signal going to the stepper driver to be switched off. This allows me to do a test cut and read the voltage on the Proma SD without it being able to adjust the Z axis.
- THC On/Off. I connected a relay to an output on the controller and it switches the + 50:1 voltage going to the Proma SD on and off. This allows me to turn the THC on and off. I am hoping to implement this as the THC on/off function in UCCNC (or I could put it in sheetcam). Now that I have an axbb-e I can control this relay synchronously in UCCNC.

I need to put more thought into how to best integrate these into UCCNC/Sheetcam Post.

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 1122
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Looking for some help dialing in a Proma SD on a new machine

Post by robertspark » Fri Jul 31, 2020 1:35 pm

xnaron wrote:
Fri Jul 31, 2020 11:49 am
robertspark wrote:
Sat Jul 18, 2020 11:46 am

I was thinking about maybe having a go at a uccnc plugin thc this afternoon (I don't have need for one but I did wonder about bringing the cost of thc down via a simple plugin comparator board for the axbbe or uc400eth or uc300eth).... the cost below that of the minithc and the price avhc as the display and twiddly knobs are not required

I have used a lot of breakout boards in the past .... any CNC lpt board will do (I have a ud1 from cncroom and a uc1 too
The axbb-e has an analog input for 0 to 5 volts. I wonder if it could be used to monitor the voltage by a UCCNC plugin?

it will not be quick enough as the read frequency is about 50hz (from memory!!!)
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 1:52 pm

robertspark wrote:
Fri Jul 31, 2020 1:35 pm

it will not be quick enough as the read frequency is about 50hz (from memory!!!)
What about using the same board (thcad-5) that they use with LinuxCNC http://store.mesanet.com/index.php?rout ... ch=thcad-5

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 1122
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Looking for some help dialing in a Proma SD on a new machine

Post by robertspark » Fri Jul 31, 2020 2:05 pm

xnaron wrote:
Fri Jul 31, 2020 1:52 pm
robertspark wrote:
Fri Jul 31, 2020 1:35 pm

it will not be quick enough as the read frequency is about 50hz (from memory!!!)
What about using the same board (thcad-5) that they use with LinuxCNC http://store.mesanet.com/index.php?rout ... ch=thcad-5
I asked cncdrive about adding that a long time ago and it was turned down as they already do THC, just via up,dn and OK signals.
http://www.forum.cncdrive.com/viewtopic ... HCAD#p5178
http://www.forum.cncdrive.com/viewtopic ... CAD#p17894

I am working on my THC and getting the development board sorted. I was getting distracted by adding ARCOK to it but I can always add that later as it is not applicable to most cnc compatible THC's anyway.
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 3:34 pm

I'm looking forward to seeing what you come up with.

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 5:04 pm

I have installed your M1031 macro and modified my sheetcam post processor to use it instead of G31. I ran a test job without THC and Torch and it worked as expected.

I have my THC configured as in the picture below.

Port 1, Pin 3 is the relay that turns on and off to 50:1 voltage that goes to the Proma SD
Port 2, Pin 4 is the ARC OK input from the Powermax 65

-THC Max and Min should not be applicable with the Proma SD
-THC Delay I know what this does from reading the manual but am unsure of whether the default 0.3 is appropriate for my setup and whether I should enable
- Anti Dive Should I set this to the relay that controls the 50:1 voltage into the Proma SD?
- Anti Down Should I set this to the relay that controls the 50:1 voltage into the Proma SD?

Maybe I should just keep it simple and use a sheetcam path rule to turn off the THC using the M11/M10 command.
20200731_140232.jpg

You do not have access to view or download this file.
Become a Contributing Member to gain access to this feature. Click Here


xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 5:43 pm

@robertspark I just re-read your post viewtopic.php?f=4&t=30670&start=100#p187017 I can use the anti dive % with a code snippet in sheetcam that can drop the feedrate. A lot to learn here... Do you have a default set of code snippets/path rules and post processor that use on all jobs or do you find you need to tweak depending on the paths for the specific job and materials?

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 8:57 pm

@robertspark thanks for the UCCNC macro and other help! This cut used your macro.



Fingernail cleanup
20200731_182928.jpg
20200731_182859.jpg


Before cleanup
20200731_182702.jpg
20200731_182655.jpg

You do not have access to view or download this file.
Become a Contributing Member to gain access to this feature. Click Here


User avatar
djreiswig
Elite Contributing Member
Elite Contributing Member
Posts: 913
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Looking for some help dialing in a Proma SD on a new machine

Post by djreiswig » Fri Jul 31, 2020 9:42 pm

Just an observation from your video. It's generally recommended to attach the work lead directly to the material versus the slats. Might help you avoid issues in the future.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 9:47 pm

djreiswig wrote:
Fri Jul 31, 2020 9:42 pm
Just an observation from your video. It's generally recommended to attach the work lead directly to the material versus the slats. Might help you avoid issues in the future.
I do that with larger pieces but find it challenging with smaller pieces like this one. I was thinking of trying a magnetic ground clamp or some other type of clamp. How do you clamp to smaller pieces like this?

User avatar
djreiswig
Elite Contributing Member
Elite Contributing Member
Posts: 913
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Looking for some help dialing in a Proma SD on a new machine

Post by djreiswig » Fri Jul 31, 2020 9:50 pm

I use a switchable magnet exclusively. Except on stainless, that is. Then I clamp a vise grips to it and attach the magnet to that.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 10:13 pm

djreiswig wrote:
Fri Jul 31, 2020 9:50 pm
I use a switchable magnet exclusively. Except on stainless, that is. Then I clamp a vise grips to it and attach the magnet to that.
Like this
Annotation 2020-07-31 201426.png

You do not have access to view or download this file.
Become a Contributing Member to gain access to this feature. Click Here


User avatar
djreiswig
Elite Contributing Member
Elite Contributing Member
Posts: 913
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Looking for some help dialing in a Proma SD on a new machine

Post by djreiswig » Fri Jul 31, 2020 10:17 pm

Yup. I think I have a 200 amp one.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Fri Jul 31, 2020 10:26 pm

djreiswig wrote:
Fri Jul 31, 2020 10:17 pm
Yup. I think I have a 200 amp one.
Thanks I ordered the 300amp one as it is the only one I could find on my amazon.

User avatar
djreiswig
Elite Contributing Member
Elite Contributing Member
Posts: 913
Joined: Thu Nov 19, 2015 10:02 pm
Location: SE Nebraska

Re: Looking for some help dialing in a Proma SD on a new machine

Post by djreiswig » Fri Jul 31, 2020 10:36 pm

I think you'll really like it.
2014 Bulltear (StarLab) 4x8
C&CNC EtherCut
Mach3, SheetCam, Draftsight
Hypertherm PM65
Oxy/Acetylene Flame Torch
Pneumatic Plate Marker, Ohmic, 10 inch Rotary Chuck (in progress)

xnaron
Posts: 131
Joined: Sun Jun 28, 2020 2:23 pm

Re: Looking for some help dialing in a Proma SD on a new machine

Post by xnaron » Sun Aug 02, 2020 3:53 pm

Here is my second cut with 65 amp consumables. Book settings for 1/4" mild steel. The cut is clean on top and the corners are nice on the top. The bottom the corners are rounder in the intricate bit. Not sure how much better I can hope for. Maybe if I slow it down a bit it will give the torch time to catch up.



robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 1122
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Looking for some help dialing in a Proma SD on a new machine

Post by robertspark » Sun Aug 02, 2020 5:11 pm

xnaron wrote:
Sun Aug 02, 2020 3:53 pm
Here is my second cut with 65 amp consumables. Book settings for 1/4" mild steel. The cut is clean on top and the corners are nice on the top. The bottom the corners are rounder in the intricate bit. Not sure how much better I can hope for. Maybe if I slow it down a bit it will give the torch time to catch up.
Try changing you corner error max tolerance to make it smaller.

I also use the following is sheetcam for uccnc (I had issues with circles at one point, so use post.ARC_SEGMENTS so that there are no issues with a complete circle any more.

Code: Select all

function OnInit()

   post.SetCommentChars ("()", "[]")  --make sure ( and ) characters do not appear in system text
   post.Text (" (Filename: ", fileName, ")\n")
   post.Text (" (Post processor: ", postName, ")\n")
   post.Text (" (Date: ", date, ")\n")
   if(scale == metric) then
      post.Text (" G21 (Units: Metric)\n") --metric mode
   else
      post.Text (" G20 (Units: Inches)\n") --inch mode
   end
   post.Text (" G17 G40 G49 G50 G64\n G69\n G80 G90 G94\n M205 (THCON)\n F1\n S1\n")
   post.SetOptions(post.ARC_SEGMENTS) --break circles or arcs into quadrants
   bigArcs = 1 --stitch arc segments together
   minArcSize = 0.1 --arcs smaller than this are converted to moves
end
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

Post Reply

Return to “Plasma Cut Quality Forum”

Industry Pros use FastCut CNC