AutoCaD to G-code/CAM

[droddis]

I have created my drawings i would like to cut on autocad 2004. but i am having trouble getting them onto a cam program or to gcode.

I will be cutting onto 6mm perspex, there are 3 layers on the drawing,

6mm cut
3mm cut
engrave

I have the drawing in both 2D and 3D. But dont know how to get any further.

I will need to do the "cut 6mm" and "cut 3mm" first, then remove the item to spray it and then put it back onto the router to do the final engrave.

I have attached one of the panel drawings for reference, does anyone know the easiest way to do this.

Also will i be ok cutting and engraving these with a dremel or not??

Hope this is enough information, If not please dont hesitate to ask.

Thanks
David

[ger21]

You need a 2D CAM program that does pocketing, like VCarve Pro or SheetCAM. Get rid of the hatch, make everything closed polylines, and save as v12 .dxf

A free alternative is to use the AutoCAD macro I wrote, http://home.comcast.net/~cncwoodwork.../AC2GCv039.zip

You'll need to draw the actual toolpaths with polylines. It will export g-code directly from AutoCAD.

[neilw20]

1.) How do you intend to do the square corners?
2.) Learning enough gcode to do this is easier than mastering a CAM package.
but a CAM package would sure make the text easier to do.
3.) The addon for Mach3 looks interesting. I will try it.

[droddis]

Will my a machine not cut square corners???

if not i supose i'll have to get my file out and get some sore arms.

thanks

[Tony Mac]

Hi David,

We have customers doing similar work and samples of their projects can be seen on the Vectric Forum at,

http://vectric.com/forum/viewtopic.php?t=2439

http://vectric.com/forum/viewtopic.php?t=2348

http://vectric.com/forum/viewforum.php?f=5

I hope this migh help and good luck with the project.

Tony

[droddis]

WOW i hope my engraving comes out that good, doubt it will. my machine isnt looking to good at the minute. I'm just waiting for my hobbycnc board and motors then i can give it a try.

Are the panels of a proffesional machine, they look like they are.

Thanks David

[under-dog]

Originally Posted by droddis Will my a machine not cut square corners??? if not i supose i'll have to get my file out and get some sore arms. thanks

With a CNC doing contouring or pocketing 2.5 D you can absolutely cut "sharp" outer corners.

Your inner, sidewall corners, however, will always have a fillet to some degree. Keep in mind that the end mill (or even ball or bullnose) you use, no matter how small, will have a radius to it. You can as an option use an insanely small endmill to finish out the corners to get as close as you can to a "sharp corner". If you deem this necissary

[under-dog]

Just actually looked at your fileCan I assume that this is some sort of control panel and that the rectangles in the middle are for buttons or lights or something

The 6mm deep rectangles in the middle will have fillets in the corners.

Are they pierced all the way through?


I am making alot of assumptions about the part in what follows:


If pierced all the way though you do not need to pocket them In this caseif it were me I would opt to coutour with an offset to the inside of the toolpath lines, with a fairly small cutter so I had a very tiny fillet. At 6 mm on a small cutter though you will need something with a long flute area.

I can assume you will need some clearence too so with the comco of the small radius and the offset you may be able to make it work without filing. Especially since I am sure some sort of button will have its own fillets as well.



If the are not all the way through then you need to pocket. In this case I would poceket it wil a larger mill and then do the small mill to clean out the corners.

[droddis]

You are right in assuming they are control panels, and i have another 50+ designs. I'm trying to replicate a 737 cockpit.

The holes do go all through except the ones on the cut 3mm layer which only go half way.

so if i understand correctly.

I need to contour the rectangles inside the line.
I need to pocket the layer cut 3mm.
and need to contour the outside the line on the edge of the object.
Then engrave.

Thanks
David

[droddis]

I've had a go with a cam program, and produced a g-code (i think).

I'll attach it and see if i'm on the right track.

I ran the code on cncsimulator and it all worked except the holes inside the pockets, and the engraving because i didn't try and program it.

I had a few problems when it was asking me to enter tools and speeds, as number one i have no bits at the moment. number two i have no dremel so i dont have any speeds.

Is this right or am i way off here.

Thanks
David

[Switcher]

Just delete the speed & tool number If not needed, after the g-code is created?

[under-dog]

Originally Posted by droddis You are right in assuming they are control panels, and i have another 50+ designs. I'm trying to replicate a 737 cockpit. The holes do go all through except the ones on the cut 3mm layer which only go half way. so if i understand correctly. I need to contour the rectangles inside the line. I need to pocket the layer cut 3mm. and need to contour the outside the line on the edge of the object. Then engrave. Thanks David

Yes

The best way to think about this is:

Contouring just follows the geometry fron your cad design literally (you can designante offsets etc) but in the end it just follows your lines. So it workes well for cutting out things but can have the effect of pocketing if you do not cut all the way through. I will elaborate after I explain pocketing. Contouring can use open geometry as well as closed geometry so it can cut just a straight line not just a circle or similar closed off paths.
I will elaborate after I explain pocketing.


Pocketing views your geometry as boundries which it will cut up to so not only will it follow your geometry (up to your lines) but will core out al the material in between. It needs to be closed geometry.


So as an example here are 3 ways to use a circle:

1) Contour all the way through the material - you get a circular through hole

2) Contour but not all the way through - you get a donut shaped "pocket" that is the thickness of your cutter. This is where i mentioned it can give the effect of pocketing. It is good to do where you need a slot or feature that is the width of an existing cutter as it will machine much faster than pocekting. Pocketing traces the border then removes fron the middle. This just makes a series of passes along your path.

3) Pocket - you get a circular sahped pocket to your specified depth



To pocket your rectangles in your center would work but.... be a waste of time and material as it literally removed (as chips) all of the internal material. Alot more unecissary lines of code to run as it cores the middle out. Contouring will just cut out the center much like you would with a coping saw, leaving a small rectangle of scrap in the center