[Bigrhamr]

I've got a table using DT electronics and am trying to learn how to operate it (better). My previous CNC experience was with PlasmaCam so I never really needed to know what I was doing, just load the drawing and push the button.
Now most of the parts I cut have been exported from PlasmaCam in G-code and DXF. When I open the G-code in Dynatorch software I have all G01 moves with no G02 or G03. If I use the DXF-Gcode converter I get the same thing. I've been fumbling around cutting with mediocre results and lots of errors until I loaded some different files with G02 and 3 moves and they cut great. It looks like I'll be getting some different software, looking into WeCim now. Until then does anybody have any ideas what I can do to use the files from PlasmaCam?

Thanks for any help.

[magma-joe]

Bigrhamr,

Each CNC machine whether it be a plasam table, mill, lathe router or what ever has its own unique CAM software "Post". The Post tells the software to export G code for that particular machine. I suspect that G code output for a Plasma Cam is different than what is required to run a Dynatorch properly.

To have any chance of cutting your Plasma Cam G code files you need to convert them back to DXF files and then run them through the Dynatorch DXF file converter or We-cim for the proper Dynatorch G code output.

Do you still have access to the Plasma Cam software and the drawings? You will need it to change the files back to DXF. Make sure you delete any lead ins or lead outs that the Plasma Cam software added when you save the files back to DXF. The drawings must be clean. New leads will be generated in the Dynatorch G code converter. I have a friend with a Plasma Cam and who has given me DXF files for my Dynatorch before which I have run through We-cim. He had to clean them up and save them to DXF before I could cut them.

Magma-joe

[Bigrhamr]

Magma-joe,

Thanks for the reply.
I do have access to the Pcam software. I have been playing with the arc resolution and allowable arc deviation settings in Pcam and exporting as a DXF. Now I've been able to open them in the DT DXF converter and get the
G02 and G03 codes, but with some loss of resolution in the arcs.

I've got a few questions, first you mentioned the DT DXF converter generating lead ins. Mine does not seem to create lead ins, is there something in setup to make that happen?

Second can you confirm my thinking that I want the G02 and G03 arcs whenever possible as opposed to many short straight lines?

And last if you are using We-cim is it all it's cracked up to be? Looks very impressive in the online demos but I'm wondering how user friendly it is. Any comments about it plus or minus? Opinions on the learning curve?

Oh and I should mention I have the 3.2 software, do you have it or the newer version?

Thanks and Happy New Years.

[magma-joe]

Bigrhamr,

Oops, I so rarely use the Dynatorch DXF file converter I had forgoten that it does NOT add lead ins. We-cim can add user definable leads if you desire. The only time I use the Dynatorch DXF converter is when I am at the machine and want to cut a bracket from the Dynatorch Plasma Mate program.
The Plasma Mate files include lead ins.

Otherwise, all my CAD CAM work is done on the computer in my office. I save the files to a USB thumb drive and carry it to the machine to load. I use We-cim to process my drawings to G code.

I would agree with your conclusion about more arcs are better than straight line segments however your ability to process these drawings is dependent apon the capabilities of the CAM software you are using. I can tell you that although the Dynatorch DXF converter works well, it is basic program.

We-cim is professional level software with all the bells and whistles. In a manufacturing enviroment its ability to track materials or nest a whole sheet with a keystroke are mandatory features. Other features like automatic kerf compensation, user definable lead ins, lead outs, multiple tool library for different nozzel sizes or for the Dynatorch Scribe are features that any user needs to make consistent quality cuts.

The Cutting Shop software that is included with We-cim is also a very powerful program for manipulating drawings as well as converting scanned drawings to DXF files for cutting. At this point I don't know how I would make it with out We-cim and Cutting Shop.

The learning curve all depends on your current level of knowlege. When I started I had never owned a CNC machine. I was definitly overwhelmed at first but like anything else the more time you spend working with it the faster you pick it up. Dynatorch does offer training classes as well as Wittlock Engineering offers phone support whereby they remotely control your computer screen and give you a training session while on the phone.

Magma-joe

[Edwardo]

Good morning and Happy New Years to all.

I am the same as Magma-Joe, i havent used the converter since i was first learning how to run my DT, another option is Sheet-cam, if you can get your PC files back to .dxf and like Joe said, remove lead ins/outs then Sheet-cam will convert your files, and use the DT post processor included in Sheet-cam.
Sheet-cam has auto leadins/outs, kerf compensation amongst many other features, once i post process my .dxf files in Sheet-cam, it saves that file as a .tap file... and the .tap file imports directly into my DT and is ready to cut.
Just another option.

EDD

[WSS]

bigrhamr,

I am new to both windows and CNC, I am using we-cim and am happy with it. They just released V19 a couple days ago, so you would get the latest version if you purchased now (It looks like there is an upgrade fee for DT users).

The online help from Gary is tops. He wrote the software and is good at explaining what's happening.

DT has a quick start video for we-cim that lays out the basics.

[ame="http://www.youtube.com/watch?v=OICiqh-293I&feature=player_embedded"]YouTube- WeCIM Tutorial[/ame]

Happy New year!

WSS

[Bigrhamr]

Thanks for the input guys, I've downloaded the trial version of SheetCam and it seems pretty straightforward to use. We-cim looks like it has a lot more capability and I do need something to use for raster-vector conversion. Does anybody know if they offer a trial version?

Now here's another newby issue I'm trying to wrap my brain around. If you are using the "slow at vertex" function in the Dynatorch software does it only see the relationship between 2 adjoining lines of code? For example if I have a drawing of a jagged tree made up of all short lines and no arcs the machine would not slow at the corners if the angle between each short line does not exceed the angle threshold I have set, even though it may be doing some high g-force direction changes. Make sense?

Now that I'm getting arcs in my drawings the slow at radius function takes care of that but I'm just trying to make sure I understand what is happening as I make changes.

[LeonD]

Hi again. I just happened to be in the "zone" and saw your message. Several notes; Arcs are better arcs than lines making arcs. Many art libraries are created with programs like Corel. When saved as a DXF these programs only output lines. No arcs. All arcs are broken into many small lines resulting in poor quality when cut. When converted directly, they stay lines. Programs like Wecim can identify what would work better as an arc when doing the offsets for kerf and will output arcs again. Always preferred.

Second, you are correct. The program looks ahead to the next line. If using lots of very short lines, the slowdown does not have time to correct on the fly. A very short line before a sudden directon change will not allow the system to decellerate. The higher the cut speed the more this appears. Also note that the vertex slowdown degress in non-linear. As the number increases approaching 90 degrees, the effect is more dramatic. As for curves, the radus factor handles that. Lower is slower. Default is 1.2 but numbers below 1 will be dramatic.

Hope that helps.

[Bigrhamr]

After calling Gary and pestering him with endless questions and getting an excellent online demo I bit the bullet and ordered WeCim with the cutting shop version 3. Can't wait to get it, looks like it will make life a lot easier (and more productive).

[magma-joe]

Bigrhamr,

I think you will be very happy with the We-cim software. It is a great package for the price when you consider the Arbor Image cutting shop raster to vector software is included.

Magma-joe