Please Help with a Macro for sheet cam

[vatso]

Hi all,

Just quickly love this forum and community. I have an issue where my compressor can't keep up with my home made plasma cutter.

I am running a 2.2KW belt driven compressor with 115Lt tank vertical type due to space restrictions I have.
I also run a hypertherm 65 which is an air eater

So what I want to do is the following I am just not sure how to do it? I am really stupid when it comes to this so I need an idiots guide to making this work? could this work on in Path Rules in sheet cam?

"The poor mans way is to write a short code snip in SheetCAM that lifts the torch and does either a long pause (G04 P 300 = 5 minutes) or an M00 (pause until you get a Cycle start) and insert it in your cut process list."

I can insert the code into the tool path I think I would do it just before the M03 code. there would be 2 options one being put it before every M03 for like 30 seconds and or every few parts and let it wait for 2 to 3 minutes? It would depend on the parts and length of the longest cut but I will work that out

Thanks in advance for the help

Mark

[vatso]

I think I found a solution there is a setting with a delay after cutting in sheetcam I am using the only issue is that it runs after every cut which is not great when one has lots of detail. I think I will try just input the delay g-code unless there is a smarter way to do this?

thanks
Mark

[Capstone]

I'll bump this thread up a bit for input as well. I have a PM45 and a 60gal 5hp single stage compressor. When I am running a large job, I get a little concerned about a CFM drop the longer the job lasts. It would certainly be nice to insert a macro, as Mark originally suggests, to give smaller compressors a chance to catch up without having to interrupt the G-Code manually.

Anyone know how to do this as a snippet to possibly auto-sync this to any based on how long the job is without having to manually insert it?

[acourtjester]

It sounds like you want a delay so you can give the compressor time to catch up you can use a manual delay M00 this will stop mach until you hit run again. I just don't know how you would insert it in the G-code where you want it. you may need to edit your post processor for this to at the start of a new part cut.

[tcaudle]

Break your SheetCAM job up in units of work by grouping contours and assigning them to LAYERS. You can have as many groups on layers as you want, Just make sure everything on a named layer cuts the same way using the same tool. Then as you build operations (each operation is done on a layer) just insert a code snip that is an M00 (or a really long pause).
I used to do this if I had a lot of close detailed cuts that caused heat to build up and it needed to "rest". Its also handy if you have a lot pieces that may tip up so you can move the gantry out of the way (in code) and clean out the possible tip ups. There are other ways where in the POST you can keep totals of the moves and have it stop at the next cut after it exceeds the distance limit you set but ti would still be less that accurate. You have to be conversant in LUA to modify the post and you can really mess things up if you are not careful.

[beefy]

On hot days and cutting thicker metal, the fan of my plasma cutter has been on continuously while cutting. I've worried the heat is building up faster than the fans can remove it.

Such a pause feature would also be great for those who have smaller cutters that are capable of cutting a certain thickness but just can't do it for long.

It would be a fantastic feature to have in the operation itself. After so many inches of cut (user defined) a delay (user defined) is initiated after the end of that cut.

Keith.

[vatso]

I have been playing around with how to create a pause and this works - the N3050 is the line position the code is G04 P30 in Mach General config I have set G04 Dwell in ms off - so P30 is a 30 second pause I used sheetcams pause at end of cut function but I don't like where in inserts the code. so I am going to rather put the code in manually. one just needs to look for the M05 command and after that decide where you want to add the line of code.

N3050 G04 P30
@ tcaudle could you explain more in detail how to do what you are suggesting?

Just another quick question about the gcode the N numbering does it have to be in increments of 10 or can I put my code in as N3061 for example wanting to move the G04 P30 after the Z10.0000

N3050 G04 P30
N3060 G00 Z10.0000
N3070 X122.0614 Y390.5493
N3080 Z2.0000

thanks again everyone
Mark

[vmax549]

I can think of several ways to do this.

1 Mod the post and calculate the run time of the movements while cutting. IPM/inch give you the minutes. accumalate the time and when it reaches your target time then the Pendown function will add in a G4PXX (time to wait). It would work both with air consumption AND plasma machine duty cycle (% of each 10 minutes of cutting) . When it reached the target time on the next calculated Torch start just add in a G4 P xx(minutes dwell time)

Another option would be to install a pressure switch at teh air inlet of the plasma machine. Run that to an input in Mach3.

Add a piece of Code to the M3 macro to watch the input from the switch. IF it does not see the input then fire the torch. IF it does see the input then Wait until the switch turns back off THEN fire the torch.

You would use an adjustable switch the same as your compressor Pressure switch that way it is adjustable for YOUR compressor application.

You could ALSO watch the M3 ON time in Mach3 and when it adds up to the % duty cycle of the plamsa do a HOLD for the remaining time of the DUTY cycle. Then reset the TIme to zero and start over.

Just a thought, (;-) TP

[vatso]

I can think of several ways to do this.

1 Mod the post and calculate the run time of the movements while cutting. IPM/inch give you the minutes. accumalate the time and when it reaches your target time then the Pendown function will add in a G4PXX (time to wait). It would work both with air consumption AND plasma machine duty cycle (% of each 10 minutes of cutting) . When it reached the target time on the next calculated Torch start just add in a G4 P xx(minutes dwell time)

Hi Vmax549 "TP" How would this be done? how would one right the code to get this to work? would that be in sheetcam or Mach3?

Thanks
Mark

[vmax549]

HI Mark what POST are you currently using ? The process is done in sheetcam post. I can show you better than I can explain it. I can Mod your post and you can play with it . Do you know the duty cycle of your plasma machine ? or air compressor.

(;-) TP

[vmax549]

Here is a test post that does Air/plasma duty cycles. It tracks both. The code is commented so you can see what it does.

(;-) TP

[vatso]

Thank you so so much

Mark