Simple CNC flywheel milling

[cfellows]

Here's a video of a simple technique for cutting the spokes in a flywheel. I developed the G-Code to cut the pattern for one space between spokes. After making one pass for one space, the g-code stops and I manually rotate the rotary table 1/6th turn. Then I run the g-code again to make one pass on the second wedge. This is repeated until all 6 spaces have one pass. I could complete the flywheel by repeating the 6 sections with the z-axis lowered. By doing this enough times, I would cut all six sections free.

However, I will modify the g-code to loop so I can make multiple passes on one section until it is cut thru. Then I'll manually move the rotary table 1/6th turn and repeat the g-code loop. After 6 times, I'll have all the sections cut through.

[ame]https://www.youtube.com/watch?v=iDAtJ_oH8dk[/ame]

The advantage of this method is the g-code is extremely simple and doesn't require CAM. The original wedge shape was laid out in Visio.

Chuck

 

[kvom]

One of the advantages of having a CNC mill is not needing to use a rotab for jobs like this. With a simple CAM program you could mill the entire job hands-off, and no need to center the workpiece on the rotab either. For slots like this it's useful to ramp the tool down, avoiding plunging at the start of a cut; plunging tends to cut wider than the tool, esp. on thin cutters like this. However, I'm assuming this is just an exercise in learning g-code.

Assuming you are using Mach3, you could use your current program as a subroutine and rotate the coordinate system via G68, thus avoiding the need to rotate the table for each pattern.

Using a drill chuck for milling is a bad idea as I'm sure you know.

 

[cfellows]

One of the advantages of having a CNC mill is not needing to use a rotab for jobs like this. With a simple CAM program you could mill the entire job hands-off, and no need to center the workpiece on the rotab either. For slots like this it's useful to ramp the tool down, avoiding plunging at the start of a cut; plunging tends to cut wider than the tool, esp. on thin cutters like this. However, I'm assuming this is just an exercise in learning g-code.

Assuming you are using Mach3, you could use your current program as a subroutine and rotate the coordinate system via G68, thus avoiding the need to rotate the table for each pattern.

Using a drill chuck for milling is a bad idea as I'm sure you know.

Thanks for the TIP on the G68. I'll check that out. As you say, this is mostly an exercise in learning G-Code, and I'm avoiding the plunge into CAM for the moment. I'm also trying to show people who haven't made the plunge (so to speak) into CNC that you can ease into it once you have the hardware set up.

I am ramping down into the cut on the first (small) arc. As far as the drill chuck goes, yeah, I know it's not recommended, but sometimes, in the excitement of trying something new, I don't always follow the tried and true methods of work holding...

Chuck

 

[DICKEYBIRD]

Cool stuff Chuck, it's great watching the machine cut what you code isn't it!

For simple stuff, try Ace Converter, a free .dxf to G Code program.
http://www.dakeng.com/ace.html

You can draw up a simple .dxf in your favorite free CAD program, load that into ACE & boom, you're done. The program let's you choose the order of cutting using layers in CAD, set the depth of cut & how much to take off each pass, etc. It's no fancy CAM program but it's simple & free. I used it for years making r/c model airplane parts on my homemade router & it was great. I could shuffle around a bunch of parts in CAD, using every available sq. in of space on the sheet of material, add lightening holes, etc. and ACE would spit out the code on seconds.

I think Mach's LazyCam does .dxf conversion as well but I haven't tried it yet.

 

[ddmckee54]

Chuck:

I used Ace converter for years and was very happy with it, then I got Cut2d. That was $150 well spent, I wish I had done it years ago. I applaud your wanting to do it the hard way and learn the G-codes. However if you really want to make chips, get the conversion software and let the "High speed moron" do the conversion. Use the creative juices for the design and let the software figure out how to get the machine from point A to point B, it's much less frustrating.

Trust me - been there, done that , got the tee-shirt.
Don

 

[cfellows]

Cool stuff Chuck, it's great watching the machine cut what you code isn't it!

For simple stuff, try Ace Converter, a free .dxf to G Code program.
http://www.dakeng.com/ace.html

You can draw up a simple .dxf in your favorite free CAD program, load that into ACE & boom, you're done. The program let's you choose the order of cutting using layers in CAD, set the depth of cut & how much to take off each pass, etc. It's no fancy CAM program but it's simple & free. I used it for years making r/c model airplane parts on my homemade router & it was great. I could shuffle around a bunch of parts in CAD, using every available sq. in of space on the sheet of material, add lightening holes, etc. and ACE would spit out the code on seconds.

I think Mach's LazyCam does .dxf conversion as well but I haven't tried it yet.

Yeah, there's something primal about the whole process... especially the precision that CNC gives to the cut. Thanks for the tip on Ace, but I've downloaded the CAMBAM demo software and it's pretty easy to use, so I think I'll just buy it.

 

[cfellows]

Chuck:

I used Ace converter for years and was very happy with it, then I got Cut2d. That was $150 well spent, I wish I had done it years ago. I applaud your wanting to do it the hard way and learn the G-codes. However if you really want to make chips, get the conversion software and let the "High speed moron" do the conversion. Use the creative juices for the design and let the software figure out how to get the machine from point A to point B, it's much less frustrating.

Trust me - been there, done that , got the tee-shirt.
Don

I took a class on VCARVE PRO which I think also developed CUT2D. But for the money, I think CAMBAM will do the trick for me.

 

[cfellows]

Following KVOM's advice, I enhanced the G-Code to cut the entire flywheel center automatically. I added a loop which executes 6 times and used the G68 code to rotate the Coordinate system 60 degrees between iterations. This then cut all six spoke openings without any intervention from me (other than manning the shop vac to keep the chips cleared). Here's a picture of the machined flywheel center.

For those that are interested, here is the g-code I wrote.

% (Flywheel Program)
(0,0 is at flywheel center)
G1 x-0.0469 Y0 F8
#100 = 0
M98 P0004 L9
G1 X0 Y0 Z.02 F8
M98 P0002 L6
G69
M30
O0002 (Rotate Coordinate System)
#100 = 0
M98 P0003 L9
G1 Z .02
G1 X0 Y0 F8
G68 X0 Y0 R60 I1
G1 Z .02
G1 X0 Y0 F8
M99
O0003 (Cut Spoke Opening Subroutine)
#100 = [#100 - .030]
G1 X0.1771 Y0.476 F4
G3 X0.3171 Y0.3933 Z#100 I0.1454 J0
G1 X1.2871 Y0.9502
G3 X1.3095 Y1.0937 I-0.049 J0.081
G3 X0.2732 Y1.6826 I-1.31 J-1.094
G3 X0.1771 Y1.5893 I-0.003 J-0.093
G1 X0.1771 Y0.476
M99
O0004 (Bore Center Hole)
#100 = [#100 - .03]
G3 X-0.0469 Y0 Z#100 I0.0469 J0 F4
M99
%


I'll do the rest of the work on my lathe.

Chuck

 

[tornitore45]

Did you have any problem with breaking through?
I would leave the last 0.015" web and hammer it out.

 

[kvom]

Using CamBam, you could use tabs to retain the cutouts. After breaking/cutting them, file off the nubs. That's my usual approach for parts like this.

Of course, you can also define them as pockets and turn them into swarf. Takes longer of course.

 

[cfellows]

Did you have any problem with breaking through?
I would leave the last 0.015" web and hammer it out.

The last part to cut through was the radius next to the hub. I just used a pencil and pushed the cut off away from the cutter bit as it separated and fell through to the milling table.

Last night I downloaded CAMBAM and began playing with it. Seems extremely simple and intuitive to use, unlike some of the other CAM software I've tried. I also tried importing a DXF file generated by Visio and had no problem with it. The cad functionality in CAMBAM is decent. and will probably work for most 2D stuff. I plan to use up my 40 sessions before I actually pay for it.

Chuck

 

[Dave Sohlstrom]

Chuck

That is what I did when I got CamBam, use up the 40 then buy. I've had it for a couple of years now and have cut a lot of parts for the steam engine I am building for the W.T. Preston model Mike Jones (hookpilot) is building on RCgroups (scale boats). Have even done some 3D cam with it.

Dave

 

[cfellows]

Since the spoke cut-outs work so well, I decided to go ahead and finish out the flywheel.

Here's the steel pipe I used to make the rim. I sliced off 3/8" and trued up the bore, faces, and outside. I put the aluminum center in the freezer and heated up the steel rim on the gas stove. I left the aluminum OD about .006" larger than the ID of the steel rim. Once the rim was hot, the aluminum center dropped right in.

I re-ran the aluminum center thru my CNC program with a larger end mill to thin the spokes some. They are now about 3/16" thick and 3/16" wide.

CNC was only used to cutout the spokes and the center hole. All the other sizing and finish work was done on the lathe (baby steps...). I guess there is now another engine in my future. Can't let that flywheel go to waste.

Chuck

 

[Swifty]

Nice flywheel Chuck, and my favourite way of fitting things together, shrink fit.

Paul.