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

[robertspark]

there is actually a plugin in sheetcam loaded as default to create plasma tools using the chart values

[acourtjester]

One thing to remember is that the Demo version of SheetCam will only work with about 250 lines of code. And some things may not work also, it is a great program but they need to be paid for their work by buying it.

[robertspark]

One thing to remember is that the Demo version of SheetCam will only work with about 250 lines of code. .

180 lines. (I thought it was more too earlier)

https://www.sheetcam.com/downloads

[xnaron]

With small holes, the best way to manage them is to spot the hole position with a plasma drill tool as a seperate sheetcam operation and drill them manually later. At a simple level, enable pierce normally and stop when ArcOK turns on. This may need changes to your post processor. I've been able to drill out such spotted holes to M3 clearance holes with no issues (on 2mm thick material). On my plasma cutter, I now the turn the torch on for 220 milliseconds which gives a finer spot. But any shorter, the torch will not even fire. I find in 2mm I can cut clearance holes for M5 and 9mm holes to insert M6 nutserts without cleanup.

You may find some Hypertherm toolsets on the CandCNC web site.

Thanks. I will give that a try.

[xnaron]

there is actually a plugin in sheetcam loaded as default to create plasma tools using the chart values

Thanks I will check it out.

[xnaron]

One thing to remember is that the Demo version of SheetCam will only work with about 250 lines of code. .

180 lines. (I thought it was more too earlier)

https://www.sheetcam.com/downloads

Thanks I noticed that when I went to download. I am checking to make sure I keep my tests under 180.

[xnaron]

I switched mach 3 to ms vs seconds and I changed the seconds unit in sheetcam to ms. I ran another test. The torch isn't turning on when it is at pierce height. I took another video without the plasma on and you can hear the torch relay kick in at the top of the pierce height. There must be a delay in the plasma cutter (pmax 65) that I need to account for?

Reading the post from Jim Colt the timing is supposed to start when the ARC transferr relay triggers on the powermax 65. Right now Mach3 is triggering the timer at the same time as the torch on command. I need to do some more reading to see how I can configure it to start the pierce delay as soon as it sees the signal from the pmax arc transfer relay.

viewtopic.php?t=17377



Listen for torch relay

[robertspark]

have you got the transfer input wired up to your machine input?

if so you have to turn on thc in mach3 (button on mach3 plasma screenset)

or enabled via a macro you create one line of code in each to turn the thcon and off

Code: Select all

startTHC

Code: Select all

endTHC

from the M3 manual these are supposed to work but they may have been changed to the above

Code: Select all

THCon()     ' Turns on the THC
THCoff()    'Turns Off the THC

[acourtjester]

It looks like the torch is not operating as it should, It should move to the cut location drop down to find the metal surface retract to the pierce height.
when the torch fires it drops to cut height and starts cutting for each start of any cutting operation. It does not look like yours does the touch off each time, just drops to cut height and fires the torch. Here is a short video on how it should look. You will destroy your consumables it needs the pierce height to start the cut. Can you post a short G-code showing the first part of a cut operation. this G-code shows the touch off and move to pierce height then M3 fire torch next pierce delay, then drop to cut height and start cutting

G-code.JPG (83.1 KiB) Viewed 2661 times

G-code.JPG (83.1 KiB) Viewed 2661 times

[xnaron]

have you got the transfer input wired up to your machine input?

if so you have to turn on thc in mach3 (button on mach3 plasma screenset)

or enabled via a macro you create one line of code in each to turn the thcon and off

Code: Select all

startTHC

Code: Select all

endTHC

from the M3 manual these are supposed to work but they may have been changed to the above

Code: Select all

THCon()     ' Turns on the THC
THCoff()    'Turns Off the THC

Yes it was wired up however it was not being used I have a button on the screen that will turn it on and off now. I am using a screenset from another user who had removed that button. I will test again.

[xnaron]

It looks like the torch is not operating as it should, It should move to the cut location drop down to find the metal surface retract to the pierce height.
when the torch fires it drops to cut height and starts cutting for each start of any cutting operation. It does not look like yours does the touch off each time, just drops to cut height and fires the torch. Here is a short video on how it should look. You will destroy your consumables it needs the pierce height to start the cut. Can you post a short G-code showing the first part of a cut operation. this G-code shows the touch off and move to pierce height then M3 fire torch next pierce delay, then drop to cut height and start cutting
G-code.JPG

You are 100% correct and I feel stupid I did not notice that. The gcode from fusion 360 probes each time. I will have to see if there is a setting in the plasma cam post processor that will do a probe each time vs only once at the start.

[xnaron]

Sheet cam test cut 3

I resolved the issue with Mach 3 not using the Arc OK from the plasma cutter. The THC on button was removed from the screenset I was using. Also fixed is the probing now before every pierce. I used the first post processor (tom) that acourtjester linked earlier. This was by far the best cut yet from a dross point of view. The last photo shows the cut after I picked off the minimal dross with my fingernail. The holes are messy as expected as they are too small. I will try using a Plasma drill operation to spot the holes as suggested.


To do:
Check the post processor to see if it has a THC on/off spot for my M311 and M312 codes (on/off)

[acourtjester]

Great things are getting down to the finer points of your problem, so the end is near. I have another suggestion for your small hole problem and that is to use a dimpling procedure I use. At the end of this page you will see info about this procedure.
viewtopic.php?f=4&t=30244&p=183935&hilit=dimple#p183935
In the Toolset file I sent both of the tools are in that for you to try (dimpling plasma and table pause), attached is a write up on the procedure.

Dimple Operations.zip

(307.16 KiB) Downloaded 73 times

Dimple Operations.zip

(307.16 KiB) Downloaded 73 times

[xnaron]

@acourtjester - I am going to try that dimple operation too! Thanks for sharing.

I have the ability to switch my thc on and off with a Mach 3 relay using M commands. M331 - on and M332 - off. The relay switches off the input voltage to the PromaSD from the Powermx 65 50:1. Is there a way I can define these in sheetcam so it can turn off the THC when it shouldn't be on? Is this more of a function for Mach 3 to determine when to stop using the THC?

[robertspark]

sheetcam path rules

https://www.google.com/search?q=path+ru ... =641&dpr=2

in mach3, any m-code (miscellaneous / macro) except M11/M10 are non synchronous M-codes and will cause the trusty divot....

given you are running a promaSD, you could install a fast acting relay (not a solid state relay / thyristor) to cut the torch voltage to the promaSD ..... this if you had a price avhc / minithc / neuron etc would be your corner-lock or thc inhibit signal to stop the torch diving.

this relay would be controlled via the fast laser synchronous M-code M11 (to turn it on) and m10 to turn it off

thc would remain on because you still want the arc transfer signal to be sensed as if it is lost motion "should" stop (I say should as I think mach3 had that function .... I cannot remember.... so you can restart from a lost arc position and you have not wasted your part)

[xnaron]

Thank you. I have a relay installed on the torch voltage to the proma sd. Specs are:

Annotation 2020-07-14 080439.png (2.57 KiB) Viewed 2641 times

Annotation 2020-07-14 080439.png (2.57 KiB) Viewed 2641 times

Not sure if it would be fast enough. I could get a fast acting relay if its not. Due to the controller board the inputs are at 24V so I'd need to find one in that range. I'll look into M11/M10 in Mach 3.

I'm really not sure how great Mach 3 is in timing anyways. If you watch closely in my video you can see that the timing at the pierce does not seem to be consistent on each one. The pierce is 0.5 seconds so a bit hard to judge but some seem to drop to cut height faster than others. There is a bug in Mach 3 where the delay isn't very accurate for < ~1sec. The fix is supposed to be to go into the general tab and set the dwell to ms vs secs. I did this and I am not sure if it is much better.

[robertspark]

it's fast enough.

are you using an ess?

if so you setup M11/M10 in the plugin

use M10/M11 to control the relay.... note, I would wire the relay as normally closed.... so that m11 will inhibit the thc relay.

M11 has to be issued after an M3

[xnaron]

it's fast enough.

are you using an ess?

if so you setup M11/M10 in the plugin

use M10/M11 to control the relay.... note, I would wire the relay as normally closed.... so that m11 will inhibit the thc relay.

M11 has to be issued after an M3

I am using one of these https://buildyourcnc.com/item/electroni ... -USB-Board but it is made for the langmuir crossfire. The inputs/outputs are designed for 24V. I do have an ess sitting on the bench I could use but I would have to rework a bunch of things. I will look into mapping the m10/m11 in mach 3 to corresponding output on the controller.

[Rodw]

I've never used Mach but I suspect that USB could well be part of your problem which is why most use the ethernet version. 24 volt however is a good thing for greater noise immunity.

[xnaron]

I've never used Mach but I suspect that USB could well be part of your problem which is why most use the ethernet version. 24 volt however is a good thing for greater noise immunity.

That is a good point.I do have an ethernet smooth stepper I could use while I am building my new LinuxCNC controller but it would mean swapping out some 24v relay modules to 5v ones.

[xnaron]

I bought sheetcam as I can definitely see the value in it over fusion 360. It is faster and the nesting option is great. Also I liked that you could import all the hypertherm tools. Although I found that some of them did not have the correct kerf setting.

I also added my ohmic probe and did a test cut of a part from sheetcam. It worked out fantastic although I have some questions. Sheetcam project attached as well as gcode.




In the video at timestamp:

1:04 it cuts a circle and pauses about 3/4 of the way in. You can see in the pic below the issue it caused in the outline. What would cause this?

Annotation 2020-07-17 164129.png (709.57 KiB) Viewed 2619 times

Annotation 2020-07-17 164129.png (709.57 KiB) Viewed 2619 times

1:50 around this time you see it make another slight pause cutting the outline. You can see in the pic below the issue it caused in the outline. Assuming this caused by the same thing as above.

Annotation 2020-07-17 164231.png (522.13 KiB) Viewed 2619 times

Annotation 2020-07-17 164231.png (522.13 KiB) Viewed 2619 times

Otherwise I am really happy with the way it is cutting now. I have the THC set to the book values. I'm not paying much attention to the quality of the smaller holes as I should have just used a plasma drill or spot op to do those but I haven't got that far.

[robertspark]

thc off is being controlled by an S code (spindle speed) which is a non-synchronous control.... motion stops before it is implemented.

[xnaron]

thc off is being controlled by an S code (spindle speed) which is a non-synchronous control.... motion stops before it is implemented.

Thanks. Found it in the sheetcam rule.

[xnaron]

So I have no rules selected. But if I click the 3 dots besides "None" it brings up the path rules and "holes" is checked. I modified the DHTC on and off with M10P5 and M11P5 which correspond to my output relay to turn the THC on and off. However if I look at the gcode it doesn not put in the M11P5 only the M10P5. The M10P5 must be added in some other place in the sheetcam setup. I modified the DHTCon and off code snippet.


Edit1: Ahh I see they are set in the Job options. Both rules are active. However the DHTC on never gets called. Maybe I need to add a rule that puts M11P5 after every M3?

Edit2: ok it looks like the EOC Anti Dive rule was the culprit. The small holes rule doesn't get applied for some reason. I will see about creating a rule I guess to add the M11P5

[xnaron]

I added a "near pierce" rule to the EOCAnti Dive ruleset to add the call to turn the THC on after the pierce. I'm not sure if this is the right way to do it but the code looks like it should be ok to me.


Edit: learning as I go here. Maybe the right way to do it is to add the "DeactivateSignal(Output5)" (which turns on the THC) to the Mach3 m3.m1s macro? It would be nice if this logic was in one place but I am not sure a sheetcam path rule will work for this.