Does anyone currently own/operate a cnc router? I have a few questions for those of you who do:

- What file format (from Shark FX) should I export to in order to generate the correct tool paths?

- If I need to cut multiple parts from one panel, do I lay them out myself into a mock up file that reflects the same size as the stock?

Basically what i'm looking for is the steps that you would take from the point the part is designed to the point the router successfully cuts the part(s).

Please advise, thanks!

Ususaly you need CAD to draw e.g. Shark/ViaCAD after that you need- CAM e.g. Smartcam

But sometimes if your router can handle and change lines to movies that you could try dwg/dxf format -But only for easy cut off.

Toolpath generation for flat panel routing is essentially 2D offset to compensate for tool diameter. dxf is usually fine, some generators recognise polyline arcs, some need them exploded to line segments. There's a pretty good free/open source CAD app (mind-blowingly good considering that one guy, Dan Heeks, pretty much did it single-handed. Respect!) and 2.5D toolpath generator called HeeksCNC that exchanges STEP (solids) with PunchCAD and is a good learning tool (lots of enthusiastic user input) in addition to being useful in its own right.
Layout onto stock sheets is called 'nesting', and that's a specialised software market in itself, because similar software is used to lay out the way that boxes are stacked onto shipping pallets, layout freight manifests, container content consolidation, all sorts of things. When you're doing it manually, the things to remember are the tool diameter, which is the amount you've got to offset components from each other, and tabs substantial enough to hold the pieces together so that they don't come free and jostle disastrously about the router and other parts while not being too onerous to separate, in addition to getting the best material utilisation from the sheet stock.

Okay,

To the OP. I use Via CAD Pro to generate model for clients as part of my business. Let's look at some points from you post and how to address them. Your in blue my replies below.

[COLOR="Blue"]Does anyone currently own/operate a cnc router? I have a few questions for those of you who do:[/COLOR]

[COLOR="Black"]Yep that fits me as work with one daily and willing be getting another one in the near future.[/COLOR]

-[COLOR="blue"] What file format (from Shark FX) should I export to in order to generate the correct tool paths?[/COLOR]

Okay now we are dealing with what your CAM program will be importing to create the G-code. Most of them can deal with .stl without any problem and for 3D models that is one of the preferred format's (though will also work with other more detailed formats, the price goes up for the CAM software for those). [COLOR="green"]So for 90% of CAM .STL will deal with 3D fine[/COLOR]

2D or 2.5D Milling can be done from .dxf .dwg and many more DEPENDING on the type of CAM software you are running. Then it is a matter of depth of cut (DOC) for a given cutting operation.

[COLOR="Blue"]- If I need to cut multiple parts from one panel, do I lay them out myself into a mock up file that reflects the same size as the stock?[/COLOR]

Depends on the CAM. I use the following CAM programs (horses for courses type thing). Vectric VCarve Pro v7 (Wonderful 2/2.5D with quasi 3D effect possible and allows wide range of bits), Vectric Cut3D (allows 4 sided cutting and has a very good cutting set up), and lastly but not least CamBam Pro (allows very controlled 2.5D milling and 2 sided milling).

Two of the above program will generate true nesting of parts V Carve Pro does a better job then CamBam in my view, but both do do it and in a usable format.

[COLOR="Blue"]Basically what i'm looking for is the steps that you would take from the point the part is designed to the point the router successfully cuts the part(s).
[/COLOR]

1) Design the model and or parts
2) If Model is one of pieces set up individual model of the pieces
3) export in a format that the CAM program can use and is most effective (.dxf is less memory then a .stl file and if doing panel work will get the job done, as long as the CAM can use the file)
4) Import file into CAM program
5) Select how you want to mill the item and with which bits and such (this is where experience in milling and CNC come in and what will get the job done quickly and to the level of finish needed). This also includes setting up nesting if needed or tabs to help hold down the parts and any scrap that could come loose while milling (having a chunk of wood or plastic come flying off the machine at you is not a nice experience, luckily I have not had that issue).
6) Once you have decided on the operations and mills to do it with you generate the g-code with a proper post processor for the Control software that you are using (I use Mach3, though there are others out there just as good)
7) Set up the stock on the machine and insure that it is properly secured (whether with physical clamp downs, lateral wedging clamps or vacuum clamping) and cut it. IF you want a more detailed discussion on the Milling side there are forums that can help and I would be glad to help you set up a SOP on milling procedures for your machine.

Hopefully this layouts answers that meet your questions and also gives you the idea of how to do what you are trying to do. Good Luck

-Michael

Thanks for your very detailed response! This helps a lot. Thanks everyone – I understand now.