I see no reason why it wouldnt be. It's pretty similar.
I purchased Dolphin Cad a few months ago along with Mach3 for a CNC mill I built, and love the program. I'm now thinking of building a CNC Plasma table also using Mach3. Is dolphin Cad compatible with Mach3 for plasma?
It's been a couple of weeks since I've done anything on Dolphin cad, and thought I would ask here first. Thanks,
I see no reason why it wouldnt be. It's pretty similar.
One of the things that will surprise you is that proper cutting with plasma is more complex that most 2.5D milling and routing.
Thanks !! I will look into it.
What does a Sheetcam license cost?
I actually bought Dolphin from the advice of Harley4ever late last year.
Sheetcam seems to be directed more torwards plasma cutters. Before spending anymore money though, I would check and see if your current software would comply with what you need.
SheetCAm was written for 2D and 2.5D routing and milling. I convinced the author (Les Newell) to add in the plasma options several years ago and worked with him to get them tested.
Cost is about 170 USD. I have access to a lot of high end CAD and CAM programs. When I want to get work done I reach for CorelDraw (gasp!) and SheetCAM with a post processor for MACH.
Ok my mistake. I am wrong. But, what solution are you providing the gentlemen that is asking if his current software is usable with what he has other than suggesting to him to buy another product? A while ago when venturing into all this I spoke with a company that sold sheetcam. They were selling this with plasma cutters but sold other software for there mills. According to them, it was something they felt sheetcam was best suited for but not for milling.
Perhaps it is in semantics. The member did not indicate he was posting a toolpath out of Dolphin and used the term CAD and doing drawings. His original post was about plasma cutting and the methodology used for plasma cutting is a LOT different than simple 2D routing, engraving , or milling. If you advocate the expensive stand-alone THC approach (the "torch lifter" has all of the smarts and runs independent of the XY toolpath) so that all of the moves unique to plasma cutting are accommodated (at a steep price) then as far as the software is concerned it becomes a simple 2 axis process with the exception of when the "spindle" [torch] is fired.
If on the other hand the user would like to use the built-in THC logic in MACH3 and cut the cost of a dedicated THC (roughly $2500.00) by a factor of almost $2000 then more of the specific moves have to be in the g-code and handled by the CAM and POST. Two that are specific are IHS (touch-off sensing) with a given pierce height (based on tool table parameters) and a different (lower) initial cut height. Couple that with things like pierce delay, end of cut delay, automatic lead-ins (essential for plasma cutting), kerf offset, a CAM with those capabilites is essential.
On of the strengths of SheetCAM is it's POST processor that is a language you can program in to do more sophisticated output. A simple example is where the user can set a reference distance as a variable and it accumulates the totalized XY distance and automatically does a new Z reference before the next pierce. It prevents having to use a blanket touch off before every pierce, which on tightly organized designs results in a lot of wasted time and moves. A more complex example is where I programed a machine with multiple Z heads to look at the tool, determine which head to use, apply a variable offset in X an Y and apply those tool parameters to that head. It was on a multi use machine that could be fitted with two routers, one plasma and one router or a plasma head and separate drill.
The end choice of a lot of machine vendors is based on criteria other than functionality for the job. They tend to sell software that is something they are comfortable with (assuming they will support it); software where there are bigger margins, or just the fact it's easier (for them) to use one tool for all jobs. I don't do a lot of CNC milling and I doubt I would use SheetCAM for more sophisticated cuts but for most things like brackets and drilled plates it works fine.
If his current software will provide the flexibility to accomplish the task then spending money on another solution is redundant. If on the other hand the criteria is the user really wants to do plasma cutting and not spend all his time cleaning and replacing consumables and generating scrap, then a proper CAM program is indicated.
Dolphin CAD and Dolphin CAD/CAM may well fit his needs. It is from what I read a very capable drawing and milling/routing set of tools. I can't address the finer issues of custom post generation.
One of the things most plasma guys want to do (or end up doing) is decorative cutting that includes the ability to import all kinds of media (bitmaps, canned vector artwork,etc) and to quickly adapt that into cut files (toolpaths) that are made for plasma cutting. The ability to easily manipulate text of any font, curve it, wrap it and then weld the font object to another decorative element becomes essential if you don't want to spend hours at the computer instead of the table. So the import of AI. EPS. EMF. GIF, JPG and other non-CAD type formats and use them in a design or trace over them in layers becomes a desired feature. I realize that falls outside pure CAD and has little or no relation to machining and milling. It's more sign making and drawing/Illustration but it's a dirty fact of life in the plasma work.
It's less than sensitive of me to get up on a vendors format and advocate a competing product instead of theirs, but given the fact the user was inquiring about plasma cutting and already owns Dolphin the suggestion was based not to replace, but to augment the program.
Dolphin could be used for plasma but you will have to find your torch kerf size and create a mill tool cutter for it. use the goround command were you can set leadins and runouts. You wont have settings for pierce time and torch height can be tricky when cutting thin material. Check out the torchmate website the have lots of info and kits.
Torchmate does not run with MACH. The original post was a question about running Dolphin with MACH3 and plasma. Torchmate does have a stand-alone THC which would work with MACH (probably) if you elected to spend the $2499.00 it costs and figure out how to interface the HOLD command into MACH so the torch does not go screaming off into the cut before the pierce sequence is done.
Thanks for the answers, but I'm still not 100% if my software is sufficient for plasma.
Right now I use Dolphin Cad to make my drawings, the create contours in Dolphin CAM.
The G-code is then generated by the Post Processor that was supplied with Dolphin.
From there I send the G-code to Mach3 on my mill.
I'm not the most computer literate person, and to be honest, the most difficult part about my CNC mill build was figuring out how to draw and then send programs to my mill. The actual physical build was easy.
That's why I asked if what I already have, would be compatible for plasma, because I'm very reluctant to learn another completely different Cad, Cam, Post processor program.
I'm still strugling with what I have now, and I fear that if I start something new, I may get the two confused. (I hope I make sense)
It would be nice if I could still use the Cad portion of Dolphin, but the drawings are saved as a .DRA file, and I don't think these can be read by another program like Sheetcam.