[grogsroom]

hi jim just wanted to ask you about the lead ins and lead outs on my cnc plasma dxf files are starting their cut at the start of the lead in and cutting the lead outs , i have a hypertherm 1250 and the hypertherm phc with ohmic,i use flashcut and was wondering if you think i should switch to sheetcam,also the cuts are good on squares ,circles ,but when i cut anything fairly intricate it seems to not like it and shuts the torch off,any suggestions are great, thanks

[jimcolt]

I am not familiar with either Flashcut or Sheetcam....I can't help on this! I can suggest the best ways (from my experiences) to design lead ins and lead outs...if you show me what you are cutting!

Jim

[woodman08]

we are using dxf files and when loaded in to flashcut the plasma torch cuts the lead in to the work piece and lead out crossing the work and ruining it,seems the torch is not being told to turn off and on at the proper timing.
I have enclosed a dxf file example

Would be very interested in how the lead in and out can be changed

[jimcolt]

I don't see any lead in, lead out on the file you sent.

Jim

[woodman08]

when we cut this horse at say 6inx 6in there is 2 streaks after its done right across the bottom of the horse,not cut right through but like a scribe as the torch probably raised but did not turn off when it returned,our speed was 118 pierce delay .25 voltage 138.
we will try and send a result photo

also when i load the file i see the lead in ,i will get a screen copy and post it

[woodman08]

i cannot seem to upload the *.nc file that flashcut makes when you load a *.dxf but i feel flashcut is adding the lead ins/outs and the torch follows or maybe we have some setting on the torch wrong that its raising but not turning off.
This is happening to all files except a plain square cut or circle or star,anything more complex like a dog or horse it messes up.
I cannot get any answers yet from flashcut,but from you at least we're hearing the diagram (original)is clean
When the program finishes ,we get 2 streaks where i have shown the arrows
I checked on loading a *.dxf file and flashcut asks the size,the feedrate,the position (lowerleft) but then it asks decimal value--- join tol---- and chord error----which all
have default values (decimal_2,join tol_.002 in, chord error_.00100in)
Have not touched these values,but thats the only changes one can make before flashcut generates the code (*.nc file for it to use)
Would be nice to know what these mean and should there be an adjustment

stan

[woodman08]

the horse has a lot of cuts but its the two at the bottom ,we have been re-using material as the cost of this steel is up there

[Pandinus]

It looks to me like a milling / routing post ... turn spindle on, route the whole thing, turn spindle off.

Just had a quick look at the flashcutCNC website and it looks like a milling system... it doesn't "Look" like its meant for plasma... and plasma is not listed under applications... So it wouldn't create leadins and leadouts and pierce cuts...

for starters you can manually edit the gcode.. remove the initial M3 and add a pierce before each Z"down" ... G1 to a Z height for your pierce and then (maybe) add a G4 (Dwell) for the Pierce delay... and ad an M5 before each Z"up" to stop the torch...

to create your Gcode you could try plasma777.com and try the DXF to Gcode, but you will have to edit the "post" section a little it has a section for starting the machine (file header)... moving to the pierce(lines 1-10)...starting the cut (lines 11-20) and stopping the cut (lines 21-30)... and finally stopping the machine... (file footer)


Its a bit of a thing to learn, but its free and I have had some luck with it so far...
It has a button to "SAVE PART" but so far I have not figured out what it does..
There is a tab to select a cutting order.. you have to click close to the leadins to select the path...


for example
the header could be your homing routine

G71 (set INCHES)
G90 (Absolute distance mode)
G91.1 (Incremental arcs)


the "MOVE"

LINE001:F50 (start move FEEDRATE 50)
LINE002:G1 Z5 (move to traverse height Z5)
LINE003:
LINE004:
LINE005:
LINE006:
LINE007:
LINE008:
LINE009:
LINE010: (end Move)

It will insert a G0 move here to the pierce point.....

LINE011:F200 (start cut FEEDRATE 200)
LINE012:G1 Z0.15 (Move to pierce height Z0.15
LINE013:M3 (Turn torch on)
LINE014:G4 P0.6 (Dwell .6 seconds)
LINE015:G0 Z0.06 (move to cut height Z.06)
LINE016:
LINE017:
LINE018:
LINE019:
LINE020: (end start cut)

It will insert G1 moves to perform the cut.....

LINE021:M5 (stop cut TURN TORCH OFF)
LINE022:F100 (FEEDRATE 100)
LINE023:G1 Z1 (Raise torch)
LINE024:
LINE025:
LINE026:
LINE027:
LINE028:
LINE029:
LINE030: (end stop cut)

And the footer could be

F100 G1 Z5
G0 X96 Y48 Z5 (Move the torch out of the way for loading unloading)
M30 (stop program and rewind)


If you have an initial height switch you could add the Z zero routine to the CUT section...
If you have a THC you might need to add the command to turn it on after your pierce...
ETC ETC

[woodman08]

Have a hypertherm 1250 powermax with PHC hypertherm with ohmic for the z axis control.
The machine came with flashcut and in the setup there is flashcut milling and plasma or water .But i also feel flashcut is not the way for plasma.
We also own sheetcam but its not set up and i seem to get lost when i look at it .But i can have a quick look at the code

[Pandinus]

Well I'm kinda interested in sheetcam, haven't downloaded the demo tho.

Maybe you just need to set the post processor for flashcut to "plasma mode" then??? I don't know it or the PHC.

[Pandinus]

this says something about plasma outputs

http://www.flashcutcnc.com/downloads...6_Addendum.pdf

[woodman08]

I have been told that sheetcam is very good and easy to configure ,i tired once and did not get far,but it does have flashcut as a recognized setting in nthe setup,and i have done that thyen loading a dxf file its good to go but thats the strange next step what makes it go ,there seems to be no start ,we have the newset sheercam.
That link you sent might be a help ,will look at that as ther are 5 items that want in input before you start the cut.

Thanks agin as we're going nuts here but we are close to a perfect cut

[richardlw]

i dont know if this will help but on my mach/lazycam if the file has breaks or overlaps it will lose its mind and do very similar problems

[duraflap]

I've been using sheetcam with my cnc plasma for about one year now as well as with one of my cnc routers. I love it!! In sheet cam if my
torch drags between cuts it's because I didn't set the rapid clearance setting in the material settings menu. It's simple and very effective.
Dennis

[woodman08]

your thread might be the first clue to what we're doing wrong,maybe we're setting the rapid clearance wrong as we are getting torch drags between cuts---thanks very much now we have something new to try out

[Edwardo]

There was something wrong with the file, i took that dxf and ran it in Corel Draw3x and fixed it enough to run in sheetcam... according to what i seen the problem was in the mane part of the horse and the 2 rear hooves were to close to gether for my kerf setting so i separated them slightly..
see if you can load this one into sheetcam

EDD

[Edwardo]

Also in sheetcam, it will automatically add the lead in/outs to the drawing, you can manipulate them with the different options provided in the program like length and styles, from the photos it looks as if your torch is not shutting off during rapid moves. I forgot to mention last post that there was a box around and attached to the horse ( according to my CAD program ) so the entire horse was a inside cut and the box would have been the final outside cut. Once you get used to sheetcam you will be able to see any problems with the drawing rite away and be able to go back and fix it. Corel draw3x or 4x is a huge CAD program that took me a long time to get onto but once you figure out what you need and dont need it becomes a great tool to use IMO.

EDD

I just took your took your .dxf file and ran it the way it is in sheetcam, if its the same file for the photo of the horse you cut, sheetcam doesnt show any inside cuts, only the outside.. BTW i use 0.05 for most of my cutting with fine cut consumables.