how would i go about doing this i have 12 4 x 8 sheets im cutting 24 parts out of each sheet i have positioned in cad how i want them on a sheet but i will have to move the sheet forward and around at some point so how to i have alignment marks im new to this but i have some experience with Mach 3 on a cnc 3040 but its not like i set a x0 y0 z0 on this machine how do most people touch off per say or set their corner to x0 y0 z0
im figuring i will have to have some saw horses at the same height as the table so i cut level any help is greatly appreciated i have looked on youtube to see if anyone else has tried doing such a thing
You’ll need a couple of the roller guides supports used for table saws & such. Like this:
Those will support the sheet where it extends past the table.
Then make an L from something like 16ga steel. Do that by taking a sheet about 18-20" square. The size isn’t critical. Butt it against the Y rail and align with the edge of the table. You need to make sure the material isn’t so thick it interferes with the Y axis gantry assembly. You also want to make sure the steel is in a position you can repeat - that’s why you butt it against a couple of fixed places on the table.
Make a design that cuts 2 lines in an L shape. Path & post-process so you have a .tap file. Set the table to the limits of X & Y and set that to 0,0 in Mach3. Run the L design. It will cut out a piece of steel that will allow you to repetitively place it where the inner corner is the 0,0 that corresponds to where Mach can move the head to when jogging to the limits.
Now you can always line up the corner of the material in exactly the same position every time which is then referencable to the design’s 0,0.
1 Like
ok i understand that but when i move that corner thru to the next 2 feet and im half way cut thru 1-2 parts and it stops cause it cant reach the part of the sheet thats hanging off till i go to move it forward in how do i align that in their just wish i had something that i could make this easier to explain
You actually need to break your part design into two pieces so you can have separate tap files for each section of the material.
ok so the crossfire has a cutting area of 25.3 Inches X 23.3 inches so on my drawing i put rectangles that size do i want to break those down into individual files and what would be the easiest way to convert them to tap files or gcode i have lazy cam but im not real familiar with it to be able to convert dwg or dxf files to gcode and be confident enough in it and i found that my plasma cutter is giving me a cutting kerf of like .131 dia so im thinking everything needs a offset half of that or a bit more for sanding im an autocad guy and im finding it hard to easily convert to gcode
Have you tried Fusion 360 - it’s an Autodesk product so should be a quick learn.
I’m not Lazycam proficient so I can’t tell you how to do it in that. But for Fusion you simply create a toolpath for each set of parts. Then you use the post-processor function to generate the GCode which will be in a tap file you can run. You’ll get a separate tap file for each toolpath you generate.
Or if you generate & post-process all the toolpaths at once (if the Setup is highlighted instead of the individual toolpath) you’ll get a tap file with all the parts GCode. You can edit the GCode in the tap file and find the lines that match you toolpath names - they’re comments. Insert a pause command for say 30 seconds or a minute so it stops to let you reposition the material. You can extend the pause from the Mach3 console if you need more time. Then either wait for it to restart or do that in the console.
You’ll want your parts setup in layers so it keeps 0,0 as the starting point between toolpaths otherwise it will try to go off into space where there’s no table.
i have it and i am an Autocad guy but the system in it seems so foreign i have no idea where to start with it but it seams that’s where im having to go and not much out their step by step how to bring in a DWG and set up to cut also im finding that their is no real tool sets made default for plasma cutters in 360 but if you know of anything that might help me on my way it be great
That’s true. You’ll want to define yours in the Fusion tool library. I have several setup for various tip sizes, materials & amperages. That way you can pick the one whose presets match what your cutter does in real life. It’s worth doing a little testing with a calibration design - one with some circles & squares as well as line cuts. You can then dial in the lead-in/lead-out values, kerf, pierce time, speeds, amps, etc. and have a sample you can grab to see if things are consistent or if consumables are getting trashed.
It makes setting up toolpaths a ton easier as you can pick the tool from the library that matches the material & cuts you’re making.
BTW, my rule of thumb is to use the max amperage the tip is rated for. That eliminates one variable when setting up my cuts. There’s no advantage to running a 1mm tip at 40A for instance vs 45A but you can bump the speed up a bit. So I really only have to worry about 3 power settings - for the RW it’s for .6mm, .8mm and 1mm tips. For the Hypertherm they use “fine” and “standard”, etc instead of orifice size but it’s the same idea. 
1 Like
yeah and im having a tough time finding any kind of documentation on kerf sizes with specific consumables i hate going off of what ever i can measure hear cause what if i am having a problem and i dont know its a problem ya know what i mean i have nothing to compare to… at some point im going to make a youtube video and document how im doing all this cause i can see where others might get frustrated with learning all this
I have a 4x6 test piece I use. Once I get it dialed in with clean cuts and no top/bottom dross that’s what I use for my settings. There’s some slop in the process because there’s always new vs used consumables but I set it up using used (but not toasted 
) ones since most times they’re going to have run time on them.
It’s worth spending a Saturday doing some testing. Even though it seems to be a waste of material, it saves you time and steel later on. I also use cut-offs from my supplier for this - I can get 20 or 30 8x10 sized pieces of steel for $5 ($10 for aluminum). I use them for welding practice too 
1 Like
ok well for those that have the Hypertherm Powermax 45Xp i found this and it has most everything you need info wise[kerf etc info for HYpertherm PM 45Xp https://www.hypertherm.com/Download?fileId=HYP189352&zip=False
ok so far i have created a single tool path that cuts everything but will not maintain the order i select in fusion 360 so tried separating holes from the perimeter of the plates due to the holes needing to be specific in place and i want them cut first so as to not have a chance to be off if it were the other way around but even with them on 2 separate tool paths they still go however they want im not sure what im doing wrong but i know id always would want my holes cut first in something and not last
ok so 2 tool paths 1 with internal holes and one that is perimeter of parts and turned off preserve order and now all goes the way it should be intended
1 Like
so far so go had some miner hang ups where the torch end got caught and cut into the good part but ive slowly figured out what was wrong and have fixed most of my problems now what i see happening is that the first cut doesn’t happen the torch blows air but doesn’t cut but it gets to the second hole and will cut no difference in heights and seems to happen just about everytime
Try bumping your pierce delay up. Or manually fire the torch (F5) on & off before you tell it to start the job. Someone else mentioned they had the same issue with their torch last fall and that’s how they got around it. You could also add a single hole that you don’t really need cut and have that set as your first toolpath. Then when it doesn’t cut you don’t care because the second one is what you really want done.
1 Like