PDA

View Full Version : CNC workflow



BillH
08-17-2006, 03:27 PM
For future reference, I am trying to figure out exactly what the CNC workflow is.
Say I make a complicated 3d extrusion in Solid Works. Where do I go from there? Do I import this solid into a program like Master Cam, and does Mastercam convert this file to G-code? Does mastercam replace EMC on linux? I know you feed the g-code file to EMC. How do you configure the machine to the workpiece? Various tooling, setting 0,0,0 on the workpiece. etc. Do most 3d parts go thru multiple chuckings on the cnc mill?

plm
08-17-2006, 08:32 PM
Bill,

A general overview of workflow. . .

If you can machine the part in 2-1/2D, then from SW’s make a 2D drawing file (.slddrw) from your solid model file (.sldprt). From your 2D drawing editor, save a copy of the drawing file in a .dxf or .dwg format (these are acad formats that most CAM programs can import).

Note: try to use layers when you make your drawing file. Put title blocks, dimensions and annotations, etc. on a separate layer(s) rather than the layer that contains the lines for the geometry. If you use just one layer for everything, you will import unwanted stuff into your CAD program; you only want to import the geometry.

If the part requires 3D machining, open your .sldprt file. You can create an .iges file directly from your .sldprt file for import into your CAM program. There are other formats for 3D, but I have good luck for my stuff with .iges. You might want to experiment with the other formats to see what works well for import into MC.

After you have imported either a 2D or 3D file into your CAM program, you will have geometry that you can begin to define toolpaths for and generate gcode. Whether a 2-1/2D or 3D part, there will be a separate gcode program generated for each setup required.

Typically, the CAD program does not contain a controller for the machine; it is used to generate gcode. For any given setup, you will import into your controller the appropriate gcode file (an ascii test file) and also set the XYZ zero location.

I hope this helps.

plm

Michael Moore
08-17-2006, 08:42 PM
Bill, I've only done a couple of CNC things so far, but this is the way it has worked for a 2.5D part:

Do the 2D drawing in Rhino/Alibre/Smart Sketch/ACAD etc.

Import the DXF/Rhino/.stp etc geometry into the CAM software (Visual Mill in my case).

Select all the tools you are going to want to use, and look up the speeds/feeds/DOC that are appropriate.

Figure out in what order you are going to machine things. I like to do any drilling/roughing first, and follow that with roughing with big mills that might yank the part of the fixture, so that you can get the part back in without having to be dead on the money for a bunch of tiny features. :)

Then you just keep working your way down the sizes on the EMs towards the finishing cuts. You'll probably have to define regions to run different machining operations in - pocketing here, profiling there, drilling somewhere else.

When all that simulates good and you've tweaked what you can to get the cycle time estimate down, then you run it through the post processor to generate the txt file with the G code.

Take your tooling list and set up all the tools in their holders and measure ODs (if some may have been resharpened) and tool lengths, and load that into the machine's tool and offset library.

Mount the stock on the mill, leaving clearance around clamps, between the stock and the table/vise, etc.

Pick a tool and use it to establish part zero - this needs to match the part zero you used in the CAM software.

Load the G code and go.

However, you may want to drop the table down out of the way and watch a dry run of the first part of the program up in the air to see if it acts like it is paying attention to Z levels, part zero, not trying to drill through table etc.

Stop it, go back to zero, jack the table up, and start again. Keep a hand on the feed rate override and/or E-stop knobs in case you see something glitchy that you can stop before a crash happens.

cheers,
Michael

mochinist
08-17-2006, 09:07 PM
Michael and PLM pretty much said it all, different programmers and set up guys are going to have their own ways, but that is the basics up above. I use FeatureCam2.5d at work, and I either draw the part using FeatureCam(I can draw faster in their program than I can in Autocad) or import the drawing if I have a digital file. I know what tools I have in my shop and I have them in my tool library already, I have also set up the program to spit out speeds and feeds that both me and my cnc mill like, so I dont have to look up much or do any calculations. Next I program all the features(drilled holes, pockets, side features, etc...) I run the simulation(no dry runs for me :) ) and if I am happy with it I save and send it to the machine if not I tweak the program. Whether or not you can do the part in one setup is dependant on your part and more importantly your machine, a fourth and fifth axis make things alot easier to machine multiple surfaces in one setup.

For a simple part all this may take twenty minutes, for really complex parts I have spent 8 hours + programming.

Nick Carter
08-17-2006, 10:15 PM
Here's how it goes from Rhino>Bobcad>Taig Mill
http://www.cartertools.com/3Dpath.html

As others have commented a lot of fixturing depends on your part and your machine.



For future reference, I am trying to figure out exactly what the CNC workflow is.

BillH
08-17-2006, 10:42 PM
Thanks guys, you all cleared things up for me.