Exporting CAD Files for a CNC Controller
Creating CAD files that a CNC controller will recognize can be a very complex puzzle. Here's one example, with a few lessons learned. June 30, 2007
Question
I use a Rover 20 machine. I have AutoCAD 2000. I would like to know the way to bring my CAD drawing into Rover 20 software. I have tried saving my drawings in dxf12, but get an error message while trying to open in nc500 software.
Forum Responses
(CNC Forum)
From contributor B:
What does the error message say? Do you have dimensions or a format in the file? Dxf saves everything. Dimensions and formats will create errors even if you can't see them.
From the original questioner:
There are no dimensions or anything in the file. In fact, I tried drawing just a square, but failed. I made the square in layer P, but when importing, it says "invalid layer P". I have gone through literature and what I could make out is that dxf setup is to be done in nc500. Also assigning proper layer names in CAD.
From contributor B:
We use Woodwop and it will not let you put everything on the same layer. It requires one layer for the material size and a different layer for the part outline. Do you have the nc500 manual? Check your layer names. Correct layering is very important. Some tiny error can drive you crazy.
From Brian Personett, forum technical advisor:
Not really knowing anything about Biesse's software, it sounds like you have some issues with your layer naming. You should have documentation explaining all the layer naming conventions that it wants. Example: the perimeter of the part might be on a layer something like "Border_Z19". That defines the part as being 19mm thick. A route layer might be something like Route_Z6.35T66LF12. That tells the post that it's going to route 6.35 deep with tool 66, LH offset at a feed rate of 12 meters. What you're describing sounds like an issue with layer names.
From contributor M:
You might consider converting your drawing to G-code using an external program, not the Rover 20 software.
From the original questioner:
I am trying to figure out the naming of layers. I got the nc500 manual. One main error message I get is "U20 Error reading file".
From the original questioner:
I finally was able to get the dxf in nc500. I was trying from Autocad2000 before. This time I tried from Autocad2004. It worked. Now I have one last problem. I have 2 rover20. One has higher version of nc500. The older version has "open dxf 2D" in file menu, but the newer version hasn't… surprisingly. Can't figure out where the option is to turn that on.
From contributor N:
Nc500 uses layer names to distinguish the drawings. If the machine was installed in an English speaking country, most probably the layer names were not changed. Now the layers are as follows:
Panel is pannelo
Router is panto
From contributor N:
Which country are you from? If I know I can refer you to the right branch.
As for your problems; I think you are making the classic mistake of drawing for the sake of drawing. It means that NC500 follows a few rules:
Rule 1: the bottom left corner of your panel layer must be at coordinate 0,0,0
Rule 2: the dxf file must be generated as release 13 or lower versions of ACAD (lite would also do)
Rule 3: drawings must be polylines
From the original questioner:
I am from Sydney. The origin thing worked. I was putting the panel layer upper left corner at 0,0. Thanks for that. I am exporting in cad12. The profile I import from Corel comes as spline. And when I try to explode, it says in cad "cannot explode spline." Trying to import as it is gives error message of too many lines in nc500.
From Brian Personett, forum technical advisor:
Trace over the spline using your snaps. Once you have it traced, convert whatever you have to a pline using the pedit command.
From the original questioner:
That's exactly what I am doing right now (tracing over). It's too much work, especially for complex logos or text. Was wondering if there's a quick way.
From contributor A:
I noticed you are using ACAD 2000, so this is not a big help, but if you were using ACAD 2004 (or later), the "flatten" command will convert the spline to lines, which will convert to polylines with "Pedit" if needed. Works well for most spline entities, especially the stuff that comes out of sign making packages.
From the original questioner:
You have hit the right cord. I was a sign writer for 6 years before coming to using rover20 router for the last year. I am using autocad2004. I tried "flatten," but it says invalid command. I looked up in help also, but no such command listed. Judging by what you have written about flatten command, looks like that's what I need. Any idea where I can find that? Is it something with custom menus or something?
From contributor A:
I'm pretty sure it is in the Express tools for ACAD 2004. Load them up, and then you should not have problems finding or using the "Flatten" command.
From contributor I:
Contributor B is correct… Flatten is in the express tools in ACAD.
From contributor D:
An aside: I have given up (for now) trying to import dxf files into NC500, because I have had more success using .CID files. My application is somewhat different - I'm not trying to work from ACAD, I'm working from Pattern Systems Drill Mate. I'm posting this here as I read this thread while I was still working on using dxfs and thought the info might be useful for others working with Drill Mate.
From the original questioner:
Thanks for the help using the flatten command. I did not have express tools before, but I loaded them up form acad disk. Found the flatten command.
But... I exported Corel file as dxf. Got that in cad. Used flatten command. It converts spline to pline. Fine. Export dxf works fine and even import into my nc500 is fine. But now everything is converted to lines. I mean any curve gets broken into small line segments. This gives a jagged look to any profile. Any suggestion to fix this? Any variable to set in cad? So that curves become arc and line remains line? I know I am almost there, but only this last bit is left.
By the way, it's been so wonderful learning from so many people. Thanks to all for the valuable input.
From contributor A:
Try the following - it worked in older versions of Corel. I have not used Corel in a long, long time, so newer versions may be different. Make sure you use the option of "Convert to curves" before you export as a DXF. This will output arcs for the most part when possible for curves instead of line segments.
