Author Topic: Going over to the dark (CNC) side!  (Read 7351 times)

Offline kvom

  • Full Member
  • ****
  • Posts: 1956
Re: Going over to the dark (CNC) side!
« Reply #90 on: April 14, 2019, 12:32:06 PM »
The bi-directional feed rate is good, but for aluminum I use only climb.  That allows air blast to clear any chips and prevent welding during the non cutting move.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #91 on: April 16, 2019, 07:13:32 PM »
To finish the sandwich construction of the engine base some form of filling was needed and as I have quite a few off cuts of Corian I decided to use that rather than metal.

The sequence was much the same as the top and bottom plates but I tried out peck drilling for the 3mm holes as they were quite a bit deeper than before, I could have gone faster with the retract speed and not lifted so far out of the work, drill was running at 5000rpm.

I used a chip breaker feed for the larger holes, you can't see it that well on the video but can hear when the drill pauses the feed which if I was drilling steel or Ali would shorten the swarf, dropped down to 1000rpm on the 6mm and 7.8mm holes.

Finally machining the contour where you can see the tool ramp down and then start cutting in 2mm deep passes before it starts to get lost in the swarf which is when I stopped filiming and got the vacuum running. The 3-flute Carbide cutter romped through this at 5000rpm and 350mm/min feed.



I did not use any tabs this time as the material was thicker than needed, bottom milled off afterwards.



Quite pleased with the cut edge, no sign of cutter marks when held upto the light, this was a full depth finishing pass



I used a 50mm face cutter to thin the work down to 10mm moving the clamps to complete the ends, only downside to working with Corian is the mess.





I'll bond it all together with JB Weld but that won't be until the bearing supports have been fabricated and silver soldered to the top plate but could not resist a quick trial assembly.






Offline Admiral_dk

  • Full Member
  • ****
  • Posts: 1322
  • S°ften - Denmark
Re: Going over to the dark (CNC) side!
« Reply #92 on: April 16, 2019, 09:46:33 PM »
Nice progress so far and I like the combination of the different materials  :ThumbsUp:

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #93 on: April 18, 2019, 06:49:00 PM »
A post on another thread brought up the subject of the "Star Wheel" used on the Alyn Foundry "Sphinx" engine which is an alternative to timing gears and operated the exhaust valve on alternate strokes. A casting is supplied but I happened to mention that  it would be something worth trying to cut on the CNC. Well that was all it took to get me trying it out.

Video firstly shows the adaptive clearing, I speeded things up 20% after filming so that was a 6mm Carbide 3-flute cutter at 3600rpm, 150mm/min, full 8mm height cut with a conservative 0.25mm DOC. I went with Andrews suggestion of cutting both ways which reduced the time quite a bit. It was cutting very nicely and I did not bother with brushing on anymore suds which only seemed to make the swarf stick to the work.

There is then a clip of a 4mm dia cutter clearing further into the internal corners which went well but during the final contouring cuts it went pop which almost made me go poop. It was a cheapie and at a cut height of 2D I was probably asking for trouble. I had drawn in a corner radius of 2.1mm but that probably should have been more.

Video ends having reverted back to the 6mm cutter for the final contour cuts which I slowed down so that it would not chatter in the corners.


This pic shows the star wheel after the first clearance cuts, you can see the faceting of the curves.
 

 
This is after all the milling where the curves flow better. Interesting to see the three height bands left by the tool, although it has not done much they show the wear from the 2.5mm plate, the 1/4" flat bar and the best finish at the top which can be seen better in the video is unused edge.
 

 
All that remained was to file out the internal corners, casting shown alongside. Just need to put it away somewhere safe and resist all temptation to do more on this engine for a while.
 


Simulation of the cutting


Offline Johnmcc69

  • Full Member
  • ****
  • Posts: 454
  • Erie Pa., USA
Re: Going over to the dark (CNC) side!
« Reply #94 on: April 18, 2019, 07:03:03 PM »
 :ThumbsUp:
 Pretty cool stuff Jason! Modeling the parts, creating the program, & watching it work, is pretty exciting.

  :popcorn:

 John

Offline kvom

  • Full Member
  • ****
  • Posts: 1956
Re: Going over to the dark (CNC) side!
« Reply #95 on: April 18, 2019, 10:07:17 PM »
That is the type of part I prefer to make from stock vs. the casting as well.

Thoughts:  The big nut on top meant that your tool stick out was higher than it needed to be.  Generally you want the collet to be clamped as close to the flutes as possible and the profile cut to be as high on the flutes as possible.  4mm mill got deflected too much.

According to G-wizard, if the stickout were 12mm, a DOC of .25mm would allow a feedrate of 800mm/min in 6061 for a MRR of 1.68 cc/min.  But a DOC of 40% of tool diameter (2.4mm) with a feed of 213 mm/min has a MRR of 10.25.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #96 on: April 21, 2019, 05:26:56 PM »
Just a small item today in the form of an elliptical gland flange, used an aluminium specific cutter as they also work well in other non ferrous metals and a split point Dormer stub drill for the 2mm holes.



I cut another star wheel but took the different route of drilling 2mm holes at the root of all the internal corners which made filing to final shape a lot easier than leaving the 2mm radius from the 4mm cutter.




Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #97 on: July 04, 2019, 07:03:50 PM »
I've not had the need to do much on the KX3 over the last couple of months but thought I had better blow the dust off it and see if it (and me) could handle something a bit more complicated. I have been drawing up a 24mm bore single cylinder 4 stroke with side rods loosly based on a design published in Practical Mechanics in 1938 with the intention of CNC machining the two crankcase halves.

So with a piece of 1" 6082 T6 aluminium mounted onto a holding block I loaded up the code and let rip.

The first 3 clips in the video show the 3D adaptive clearing which was done using one of ARC's 6mm 2-flute aluminium specific HSS cutters, I was in two minds whether to use this as I had noticed a bit of chatter when using it in the manual mill in the past particularly as I wanted 27mm sticking out of the collet so that would not crash into the work but after a chat with Ketan a while back I decided to give it a go. 5000rpm, 8.5mm height of cut (1/3rd stock height) 1mm depth of cut, feed rate of 300mm per min giving achip load of 0.03mm which was just right and did not need altering. 0.5mm material left for finishing

4th clip is the same as above except height is reduced as the surface was between the two 8.5mm increments, this is where a tiny amount of chatter could be heard on the lighter loaded cutter.

Clips 5-7 are the 3D contour which was used as the sides of the crankcase all have draft angle rather than vertical sides. I used a 2-flute carbide 6mm cutter with 1.0mm corner radius. Again run at 5000rpm, with a 0.5mm stepdown and the DOC was the 0.5mm that was left, feed 400mm/min. In hindsight a 4 flute cutter would have been better as the amount of swarf was not great so the 2-flutes extra clearing capacity was not needed and then I could have fed faster.

Clip 8 Spotting the bolt holes with a 5mm HSS spotting drill at 5000rpm

Lastly drilling the 3mm holes with a Dormer A002 split point drill at 5000rpm and using a pecking cycle to clear the swarf.




The bit of flash around the bottom is due to me doing the CAM for 25mm stock but using 1" , there are a couple of things I will alter slightly for the other half but overall I'm quite pleased with how it turned out. particularly the tapered surfaces as I was expecting them to need more fettling but they are quite smooth and will just need a quick rub with emery before blasting the surface to get it to look like a casting.

Online Vixen

  • Full Member
  • ****
  • Posts: 1175
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #98 on: July 04, 2019, 09:45:44 PM »
Looks like you are getting the hang of this CNC stuff. Well done.
Remind me again who's software you are using. Is it Fusion 360 for the CAD/ CAM and Mach 3 for the machine control?
The draft angle slopes look good. Can you go curvy slopes or just straight angles?
Mike
It is the journey that matters, not the destination

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #99 on: July 05, 2019, 07:13:45 AM »
I draw with Alibre Pro and then export a STEP file into F360 to generate the code and use Mach-3 on the machine, I wanted to get the part done before Saturday so you could look it over and point out any things I could try differently.

Yes the CAM will let me do all sorts of shapes and I should probably have done a finer stepdown on the curved section under the cylinder mounting flange so will see if I can add that to teh other half.

Is this curved enough for you?


Offline Muzzer

  • Full Member
  • ****
  • Posts: 11
Re: Going over to the dark (CNC) side!
« Reply #100 on: July 05, 2019, 12:40:42 PM »
Looks pretty reasonable Jason! Takes a while to get used to creating the toolpaths, feeds and speeds, heights etc but in the end I find I can do things you simply couldn't make on a manual process and even with the extra time for programming the CAM, the overall time is a lot less for those that you could - there's considerably less faffing about with setup between ops.

One real benefit of Fusion is the fact that the CAD and CAM are closely integrated which means you can quickly and easily alternate between the CAM toolpath generation and the CAD model design and back again. The reality is that when you come to programming up the CAM, you often find you want to finesse the CAD model. Moving only one way (via STP format) is very limiting. Just saying....

One neat and powerful feature of Fusion CAM is the ability to save the part-machined output of one CAM setup as a mesh (STL) file and then reuse that as the stock for the next setup eg when you turn the part over to finish the other side. When you run the toolpath simulation, you can right click on the resulting machined stock and "save as" an STL. Then "insert" it into the CAD environment - this creates a body. When you do the next CAM setup, you can select that body as your stock and Fusion will know where what is really in front of it. Works really well and avoids "surprises".

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #101 on: July 05, 2019, 01:18:50 PM »
Thanks Murray, good to have your input which I've missed from ME

I noticed early on when watching a couple of Lars' videos that he jumped back into the CAD to make an alteration, as you say easy when it is all in one place and would be useful as the final design is tweaked. What I need to look into now is using the same set of operations for the other half which is basically a mirror image rather than having to enter them again though the practice will be good for me anyway.


I don't have any air/lube set up yet so tend to stay by the machine so probably not as productive as leaving it to it's own devices but at this stage I'm happy to watch and see if it is doing what I hoped it would. I've not yet tried anything with a second setup but may be tempted to at least do the main cavity inside the crankcase as that has no critical surfaces but either way will bore the bearing holes in the lathe with the two halves fixed together to ensure things line up 100%. It would be easier than a second setup after turning to bore the area around the cam shaft.

Offline kvom

  • Full Member
  • ****
  • Posts: 1956
Re: Going over to the dark (CNC) side!
« Reply #102 on: July 05, 2019, 01:40:49 PM »


This is called "rest" machining; you can program to the rest of the part after a roughing op.  That's something I don't have with CamBam.  One use of this feature that would be very welcome is multiple roughing passing.  Large tool to start and smaller tool afterwards, to save machine time.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6467
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #103 on: July 05, 2019, 01:45:23 PM »


This is called "rest" machining; you can program to the rest of the part after a roughing op. 

Fusion seems to do that anyway, for example on that part i first did the adaptive clearing to leave 0.5mm and then without saving or altering the setup did the 3d contour and it just removed the remaining 0.5mm, then did a couple of parallel cuts to do the flat surfaces the contour missed. Drill started from that flat surface.

EDIt, just tried it with two sizes of cutter and there is a "rest" setting that comes up when doing the clearing cuts which has option such as"from stock" or "from previous machining" but that is with the part held in the same position.

« Last Edit: July 05, 2019, 01:58:29 PM by Jasonb »

Offline jadge

  • Full Member
  • ****
  • Posts: 356
  • Cambridge, UK
Re: Going over to the dark (CNC) side!
« Reply #104 on: July 05, 2019, 05:46:51 PM »
In my CAM system, for 2.5D, it's called re-machining. The key point is that one can pocket or profile using a large cutter and then re-machine only the corners using a smaller cutter. So overall machining time is considerably less. In 3D things get rather more complicated, in name anyway. There are several operations, such as re-roughing or valley machining, that all add up to the same thing. Using a smaller cutter to remove just the material left in awkward corners or fillets.

Andrew