Author Topic: My CNC Router  (Read 1162 times)

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
My CNC Router
« on: July 01, 2025, 12:50:08 PM »
I have a CNC router, which I have used very infrequently over the last ten years or so. Like ten times. It's basically a bare bones 22" x 11" usable table machine with a Bosch Colt router for a spindle. It has microswitches for stops. It is controlled by a parallel port type controller with opto-isolated I/O and three drivers. It has the usual range of available ports. It runs on LinuxCNC.

I've mentioned the stepper driver elsewhere on the forum, when I thought I was going to have to replace it because my dedicated parallel port laptop computer had died. That was solved when I found I could use another old laptop I had. So I'm back with the original setup.

Anyway, I'd like to get more use out of it now that I'm doing hot air engine experiments. My latest use for it is for cutting out small parts for a Scotch yoke drive in aluminum .084" thick to .25" thick. Simple cutouts, not profiling. 

So far I've only done simple cutouts, nothing profiled or pocketed, and that probably will be my lot for the near future, at least with the Colt as a spindle. Minimum speed for the Colt is 8000 rpm, and max is 35000. I just use the onboard switch for speeds, and on/off. I don't have spindle control.

I have used only one type of bit, an Amana # 51471 Solid Carbide CNC Spiral 'O' Single Flute, Aluminum Cutting 1/8" Dia Up-Cut Router Bit.

I had two of those, and just broke my last one. They aren't cheap. I'm thinking about alternatives, and would appreciate suggestions.

To cut a piece of aluminum, I have been either drilling holes in an oversized blank, and screwing it down onto the sacrificial MDF router table surface, or holding it down with small square tabs of thin plywood, screwed down with wood screws as toe clamps. I have sometimes had problems with the toe clamps not holding, so prefer the direct method of holes in the blank with screws -- but it's wasteful. I'd appreciate any suggestions of a better way to go. (However, not at great expense, or complexity. DIY best)

I generate G-code with Sketch-UP and the Sketch-U-Cam add-on. I run it in LinuxCNC (V 2.5.4).

I have no homing setup presently. I do it manually, which is very time consuming, and also not very accurate. I jog the tool to about where I think it should be on the blank. I have a small X and Y allowance before the bottom left corner of the part will start cutting and then zero X and Y. I jog over to a clear area of the MDF tabletop and jog Z down to a slip of paper on the table. When it is a little hard to pull out from under the bit I zero Z.

When writing the G-code I allow a slightly thicker material thickness to allow for (I hope) complete penetration into the table top a little. This doesn't always work out because of the approximate nature of my setting up above. Sometimes the metal is pressed down into the mdf. Sometimes I'm too far through, and I cut though my tabs that are supposed to keep a completed part from coming loose and breaking the router bit.

I'd like to do better than what I have been. I know it's far from ideal. I'm open to suggestions from everyone here about basic improvements I can make that are reasonably simple and I hope inexpensive, ideally DIY, or in methodology, etc. Not things like "buy a water cooled spindle, glass scales, there's a better machine for sale on ebay, etc." -- does that make sense? What can I do that's simple to make things better.... and ideally be specific if you have a construction suggestion -- link to how to, video, or a parts recommendation.

Thanks!
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #1 on: July 01, 2025, 01:27:30 PM »
Here's a pic:

  [ You are not allowed to view attachments ]  
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #2 on: July 01, 2025, 06:39:59 PM »
This evening, I did an experiment with the CNC router. I have no more single flute bits, so I tried a cheap (5 for $20) double flute 1/8 carbide bit that I had on hand. It's a SpeTool M03008. I set the router at its slowest speed (8000 rpm) and ran it at 8 IPM and a shallow 0.020" DOC. I was cutting .250" scrap aluminum -- probably 6061-t6.

I periodically sprayed WD-40 from the can on the cut. The router cut the piece out quite cleanly, but naturally took a long time, since it was 13 passes at only 8 inches per minute. Swarf built up all over, while cutting. I need something to remove it. (Suggestions?)

  [ You are not allowed to view attachments ]  

I'm surprised the cheap two flute cutter did better than the specialty Amana single flute designed for aluminum. I'm going to work on increasing DOC -- this first trial was just an experiment to see if it would cut at all.
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline BillTodd

  • Hero Member
  • *****
  • Posts: 1173
  • Country: 00
  • Colchester Essex (where the lathes were made)
Re: My CNC Router
« Reply #3 on: July 02, 2025, 03:33:17 AM »
Rigidity, rigidity, rigidity.

Since you are cutting small parts you might get som milage out of bracing the guide rods (effectively reducing their length ) .

If you can do asymmetrically on the X it might reduce resonance in the paired rods (there is zero torsional strength in the pair  because of the bearings)

Bill

Offline Country Bubba

  • Jr. Member
  • **
  • Posts: 63
  • Country: us
  • LaGrange, GA USA
Re: My CNC Router
« Reply #4 on: July 02, 2025, 07:31:34 AM »
My first thought is your spindle speed it to slow. So I pulled up "Little Machine Shop" on line and plugged in your 1/8" 2 flute Carbide cutter and sure enough, they recommend 27500 rpm! and a feed of 55ipm!  In my experience on a less rigid machine, I tend to slow the feed down a bit, and keep the speed up.
For chip control, as you have a permeable base, I would recommend keeping a vacuum close by and apply the WD as you are. You don't want to recut the chips as it will mess with the finish and "gum up" your cutter.

https://littlemachineshop.com/mobile/speeds_feeds.php

Just one's opinion.




Art
Country Bubba

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #5 on: July 02, 2025, 11:46:18 AM »
That's a great idea, Bill! I bet 90% of what I want to do in future will be small parts. I could make up some bracing clamps that are removable. Also good idea about asymmetry!  :beer: :beer:

Thanks Country Bubba!  :beer: :beer:

I have to think about this part. I thought I'd done calculations that showed chip load around .001 but after playing with Little Machine Shop's calculator I see I was still thinking single flute, rather than the change to two flute, and my speed of 8 IPM is wrong by half for 8000 RPM.

  [ You are not allowed to view attachments ]  

All I did there was limit artificially the speed of the machine to 8000 RPM. The chipload at 16 IPM will be the recommended .001" then. I'll try doubling the speed. The mfr also gives a max depth of cut in slotting of 1/2D, which is .062" I'm presently at .020" but I'll try .032" next.

I wonder about the Little Machine Shop's calculator's results for the very high speeds you found for an 1/8" milling cutter. While it may be theoretically correct for optimal cutting, I wonder if a 1/8" mill shaft would snap under the kind of side force that would generate when slotting.

The depth of cut at that speed must be very low. I could probably snap a 1/8" dia carbide milling cutter held in a vise with my hand. Not that I would try!

But thanks for that calculator, if the other adjustments go well, I might eventually bump the router speed up a notch and the IPS to suit.

GREAT! very appreciative of any and all advice!

I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline Country Bubba

  • Jr. Member
  • **
  • Posts: 63
  • Country: us
  • LaGrange, GA USA
Re: My CNC Router
« Reply #6 on: July 02, 2025, 07:13:14 PM »
On my cnc mill (RF31 conversion) which is limited to 4000 rpm, IIRC routinely would run ~10IPM with a DOC ~.100" (Trying to boot up my old win7 machine to find my info, but looks like microstooopid had done me in again:{( It won't boot:{(
I also ran flood coolant and that makes a difference.


OK, took half an hour, but win 7 finally booted and I was able to find my toolset for the 1/8" endmill and I was running at 4000 rpm, feed of 6IPM and as I remember, played around with the DOC (Been a while since I did anything on that machine and even longer on the router for aluminum!

« Last Edit: July 02, 2025, 07:50:01 PM by Country Bubba »
Art
Country Bubba

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #7 on: July 02, 2025, 09:41:55 PM »
Thanks for that Art.  :beer: :beer: That's helpful to compare to.

I decided to try another part in the same piece of aluminum, but this time at 16 IPM instead of 8. It cut perfectly fine except for the fact that in redrawing the part I forgot to put in tabs.  :wack: Luckily I noticed it at the very last pass, and was able to stop and withdraw the spindle before the part came loose. It's still a usable part, with just a thin skrim of aluminum on part of the bottom.

So since that worked out, I added tabs to the drawing, rewrote the g-code, this time with a .032" depth of cut instead of .020". The machine got a few passes down, but got wonky at one point, so I hit e-stop, and withdrew the spindle. I'm not sure exactly what happened. I checked the flutes and didn't see any aluminum welded onto the bit.

I checked the router in the mount because I thought I might have seen it rise slightly. Seemed solid. I took it out of the mount and checked shaft play. It clicked when pushed sideways, so I'm thinking maybe the bearings have had it. Could be. It's ten years old at least, and humidity in the shop is high, plus cutting aluminum is going to be hard on router bearings.

Not sure what to do now, try to repair, or think about a better spindle. I know I said at the outset I didn't want to buy a new spindle, but now I might have to. I do have one of those little 500 watt 100VDC fan cooled motorized spindles which I use for milling on my lathe. But they seem even lighter weight than the Bosch Colt router. I wonder if they can cut the mustard for milling up to 1/4" in aluminum? They don't look too rugged.

  [ You are not allowed to view attachments ]  


I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #8 on: July 02, 2025, 10:34:38 PM »
Then there's just replacing the bearings per:

https://www.forums.woodnet.net/showthread.php?tid=7355275

Unfortunately he doesn't say what bearings it takes. Wonder if they can be upgraded?
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline RussellT

  • Hero Member
  • *****
  • Posts: 537
  • Country: gb
Re: My CNC Router
« Reply #9 on: Today at 05:36:42 AM »
Hi Steve

I think most Bosch stuff is pretty well made - so I'd be surprised if the bearings could be upgraded.

Russell
Common sense is unfortunately not as common as its name suggests.

Offline John Rudd

  • Hero Member
  • *****
  • Posts: 2534
  • Country: gb
eccentric millionaire financed by 'er indoors
Location:  Backworth Newcastle

Skype: chippiejnr

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #11 on: Today at 09:13:44 AM »
Thanks Russell.  :beer: Thanks John  :beer: I ordered a set of bearings from the site you listed. Much obliged!

I think today I'll try fitting that 500 watt spindle to the mill, just to see what it can do. I did spend some time looking at various spindles in the $100 to $300 range on Amazon, and reading reviews and it wasn't very informative. Some were DC some were VFD 3 phase, some air cooled some water cooled. Seemed like the most expensive (water cooled 2.2 kw 4 bearing w/vfd) had comments like "not much torque compared to my ________" router, or even as much torque as the reviewer's old 300 watt spindle.

So I'm curious about this 500 watt DC spindle I already have. What can it do?

When I think about this stuff, I'm thinking it's likely I will probably settle on a 1/8" 2 flute mill bit for whatever I use this machine for in future. Aluminum, not wood. Small parts. That means to me, considering the overall stiffness of the machine, a speed probably where I am now - 8000 rpm 16 IPM, and depth of cut yet to be determined.

So if that's true, an ideal spindle would be running at 8000 RPM at its peak power output, not a 24000 or higher spindle throttled down to 8000. Bearings are obviously a major consideration. Ideally I would make up a non-motorized spindle driven by a belt of some sort, and a separate motor. Is that right?
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #12 on: Today at 10:42:19 AM »
I've got plenty of high quality skate bearings (608 2RS) up to ABEC9 IRC. It wouldn't be hard to make up a spindle with some water pipe as a housing. I think I have some high quality 8mm shaft as well.

I was curious about what the RPM limit was for the skate bearings, and came across this explanation which I found quite humorous:

https://www.ahrinternational.com/Skateboard_bearings.htm
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline awemawson

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 9022
  • Country: gb
  • East Sussex, UK
Re: My CNC Router
« Reply #13 on: Today at 12:10:42 PM »
Steve, I made up a high speed spindle to use in my CNC milling machine many years back using simple bearing but it was driven by an integral air turbine (jet impinging on a small gear wheel), and I arranged it so that the air passed through the bearings downwords and kept the swarf off the workpiece. As the air was lubricated being supplied from a regulator / lubricator it not only cooled but gave the bearings a chance of survival at the very high rpms that it ran at. It's probably kicking about in a cupboard in the workshop.
Andrew Mawson
East Sussex

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #14 on: Today at 12:38:30 PM »
That's pretty cool, Andrew.  :thumbup: What did you cut with it?

That also just reminded me I picked up a little turbine spindle, used at one of the old Bernardston Gas Engine shows. Forgot I had it. It was just a curiosity to me, and cheap. Unfortunately, there's no compressed air in the shed where the cnc router is, so I can't use it. Also it's kinda small.  I don't have much of a compressor in my tiny shop near the house, either.

Right now, I'm working on getting the 500 watt spindle fitted to the CNC. Looks like the router mount fits a 70-71mm body, and my 500 watt spindle has a 52mm body. I think I'll keep the existing mount and just make a 71/52mm adapter.

I was rummaging around in my scrap box and found this big chunk of aluminum, so I don't have to cast anything:

  [ You are not allowed to view attachments ]  

I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline awemawson

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 9022
  • Country: gb
  • East Sussex, UK
Re: My CNC Router
« Reply #15 on: Today at 01:00:33 PM »
I made it for engraving lettering on labels etc - I used the smallest centre drill that I could find as the cutter.

It seems it was 20 years ago !

  [ You are not allowed to view attachments ]
 
  [ You are not allowed to view attachments ]
 
 [ You are not allowed to view attachments ]  


Andrew Mawson
East Sussex

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #16 on: Today at 03:46:43 PM »
That's really nice Andrew!  :thumbup: :thumbup: :clap:

I wonder if the one I have is for engraving? That would make sense because of the size. I'll have to dig it out and get a photo of it to post.

Meanwhile, I started in on the adapter ring for the 500 watt spindle.

  [ You are not allowed to view attachments ]  

  [ You are not allowed to view attachments ]  
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #17 on: Today at 04:14:23 PM »
Done!  :thumbup:

  [ You are not allowed to view attachments ]  
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #18 on: Today at 04:16:45 PM »
It fits!  :med:

 [ You are not allowed to view attachments ]
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #19 on: Today at 07:36:15 PM »
Uh...... first attempt @ 16 IPM 8000 RPM and .020" DOC ....not so great. For some reason it seemed to wander sideways in the cut. I think the bit was flexing. The spindle and mount were really solid and no detectable play, before or after. It managed one pass, got back on track, then took a detour again, this time into double the depth of cut, which broke it.

  [ You are not allowed to view attachments ]  



 
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg

Offline vtsteam

  • Global Moderator
  • Hero Member
  • *****
  • Posts: 6781
  • Country: us
  • Republic of Vermont
Re: My CNC Router
« Reply #20 on: Today at 07:45:41 PM »
I edited the G-code and dropped the speed down to 8 IPM from 16 IPM. I then changed to a new mill bit I just received in the mail today. Also inexpensive (5 for $20) but speced for aluminum. The others were supposedly for stainless steel (!) but they did seem to work well on aluminum on the Bosch Colt router.

Anyway, I ran the same part again with the reduced travel speed, and it cut. Looks like a decent job. Not as fast as the router, but this also was a different offcut of aluminum, and might have been a different type.

I'd say the 500 watt spindle is usable, though slower. Definitely quieter, which is a plus. Also it is DC and can be speed controlled from LinucxCNC if I figure out how to do that.

Here's the results of both the first (bottom) and second attempt:

   [ You are not allowed to view attachments ]  
I love it when a Plan B comes together!
Steve
https://www.youtube.com/watch?v=4sDubB0-REg