Half Scale 1/4HP A J Weed Engine

[Jasonb]

Although they won't remove metal at the same rate as a commercial machine they are still quite capable. I could have used it for the initial ops of sizing up the material for the bed and pedestalls so 1st ops are quite possible too. The likes of Vixen has got rid of his manual mill and does it all with his CNC.

The next parts I will be covering are steel and cast iron so it is not just the easy to cut metals that they work well on, infact my feeds and speeds are fairly similar, maybe a bit faster feed for the non ferrous.

The one downside with the KX-3 is the work envelope is smaller than my similar size X3 mill so would not want to give that up, plus I like turning the handwheels.

Oh and it is not just scratch building they can be used for, even those addicted to castings could make use of them. The patterns for the three castings were also cut on the CNC.

<a href="https://www.youtube.com/watch?v=hm0E8bSQacg" target="_blank">http://www.youtube.com/watch?v=hm0E8bSQacg</a>

[Krypto]

I also appreciate how you put your speed & feeds in the video descriptions as that is very useful information for comparison with other CNC mills.  While your exact mill was available over here for a bit, it's a big country and they are probably very thin on the ground as it doesn't seem that many were sold.  I believe Tormach sucked all the oxygen out of the room for the other small CNC vendors in the states.  In comparison, Tormach's current smallest CNC mill, roughly equivalent to the Sieg that you use, has a max spindle speed of 10000 RPM's which would probably be nice for the soft metals, but not absolutely necessary as you have demonstrated.

I also find it reassuring you don't use flood coolant for your CNC work, which is great news for me as that would be a complete pain in the butt for several reasons.  Looking forward to the rest of this engine build!

[Jasonb]

The original engines came with the two disc type crank webs as iron castings, the one I have based mine on would not turn over and one of the main reasons was that the crank had twisted at one or both of the crank pin to web joints. For this reason, I decided to make my webs from steel so that the whole crankshaft assembly could easily be silver soldered together.

The two webs were first turned, drilled and reamed 8mm on the lathe and made good use of a couple of bar ends. I used a CCGT 060208 insert to give a nice fillet to the internal corner.



The webs were then held in the 3-jaw chuck using soft jaws and the "cast" recess milled. The majority of the material was removed with a 4mm cutter using an adaptive tool path, this needed a bit of tweaking of the parameters to get the 4mm tool into the narrow gap but was done mostly by reducing the minimum cutting radius. That cutter is starting to loose it's edge I can hear a bit more noise and it left a small burr around the edge of the cut then changing to a cutter with a 1mm corner radius the bottom of the recess was finished with a horizontal path and lastly the edges of the recess done with a contour going round twice. At about 3.00 mins in you can see that the shaprper cutter removes the burr from the earlier adaptive op.



The usual methods of a full length shaft and pin with reduced ends were use to make the other bits from PGMS which was then silver soldered together before a quick clean up skim of the webs on the lathe before the middle if the crankshaft was cut away. Quite like the black oxide from heating that has been left in the recess



All seems to fit and go round as it should. I'm not going to fit a pulley on mine so just made the crankshaft on the near side a bit longer than is needed for the eccentric as it saves a bit of shelf space!



<a href="https://www.youtube.com/watch?v=UZ5pORpIRwk" target="_blank">http://www.youtube.com/watch?v=UZ5pORpIRwk</a>

[redhouseluv]

They look soooo good! Is that black primer or finish you have applied to the recesses?

[Jasonb]

It is just the oxide that formed on the crank when it was heated for soldering.

[AlexS]

I just recent see your build. Nice 3d printed part. Where did you print it?

Thanks

[Jasonb]

I have seen mention of Craftcloud on a couple of other ME forums and ended up going with them. Stainless Steel 316L along with Aluminium seem to be the most common and cost effective materials and Craftcloud offer several prices for both, they also offer DMLS which is said to have smaller layer height than SLM which most other sites do so I went with a 316L DMLS part, basic sandblasted finish

.

https://craftcloud3d.com/

[AlexS]

Thank you Jason.

[Jasonb]

The Cylinder was cut from a block of cast iron. First I machined all the faces with a Shell mill fitted with inserts intended for Aluminium leaving 1mm on the sides, top, bottom and one end. This was then held in the mill vice and the ctr of the piston and valve bores spotted before drilling the valve hole 7.8mm and reaming out to 8mm.



Transfering it over to the 4-jaw the second spot mark was clocked true, the bore opened out with a couple of different size drills and then finish bored to 20mm. A also faced off this end where the piston rod goes at the same setting to ensure it was true to the bore.



While the cylinder was an easy to hold shape I did the rest of the details - tapped holes for cylinder and valve covers, steam passage and the notch to connect that to the cylinder. The other end was almost the same except it had a 4 hole pattern for the cylinder cover.



There was also a tappe dhole for the steam inlet and two holes to connect the valve chamber to the steam passages, the outer part of these holes is tapped M4 x 0.5 and will get plugged after the shaping has been done.



It was then onto the CNC to machine the "cast" shape of the cylinder. I did this in two stages, first the teardrop shape between the two flanges with the work horizontal and then the actual flanges with it held vertically.

The first part was done with an adaptive to remove the majority of the waste, a quick horizontal to finish the top of the inlet boss, a contour to remove metal from thinner flange faces so that the final scallop path did not drive the cutter into these vertical faces at full depth which was more than the flute length.

<a href="https://www.youtube.com/watch?v=jPMgmilgQfU" target="_blank">http://www.youtube.com/watch?v=jPMgmilgQfU</a>

The "Ace of Clubs" mark you can see on the surface is the result of a tiny bit of backlash in the Z axis and is where the cutter changes from a downward cut to going back up the other side or vice versa. Probably less than 0.025mm (1thou).





I will cover the rest of the cylinder in the next update.

[redhouseluv]

I watched the whole video and have a couple of basic CNC related questions please:

1. Aside from where you have to change tooling is the enitre process fully automated i.e you can sit back and watch?
2. How do you know what you have programed will work, what is the pre-production testing? I can't imagine you stick a chunk of metal in and watch it fail?
3. Is the program complied in some way to make sure the instructions are correct?

I come from a software background hence the questions having a slant towards programing

[Jasonb]

For small items that don't take long I'll probably just watch, those that run for longer I will just go and do something else and not even in the workshop so yes it is automated and will just run the program once you press start. The CAM software gives me a time each path or group of paths will take so I know when to come back and change tools for the next op or turn off the compressor if the job is done.

As I design in Alibre and do the CAM in F360 the first thing I have to do in export from Alibre and open in F360. Then I set up my basic part, size of stock and the orientation of the stock. I also pick a datum point which is where I will locate the work on the CNC, often top ctr for me, others may use a back corner.



I'll then go on to choose which type of cuts I want to use, the cutter, feeds and speeds, depth and stepover, etc These are what are listed down the right side along with the setup. There is a second setup and paths for when the part gets turned over to do the other side. I can duplicate or copy and past the details from the first op and just alter them slightly for the second so don't have to do it all again. The path of the tool and what it will remove is shown here, Blue is when it ios cutting, yellow when moving about but not cutting.



There is also a "simulate" option where you can watch the tool as it actually cuts the material. I use a contrast which has the waste shown in purple and the finished part in green. This gives a good indication of what the tool will do. Not the length of the tool, I extended it from my default setup for this as the 4mm tool needed to reach about 20mm deep.



In the image below I have reduced the tool stickout so that it is less than the depth of cut.



If I then run the simulation it flags up any crashes, 654 in this case which are all the red marks towards the end of the progress bar at the bottom of the screen. It also shows in grey where the tool holder has come into contact with the workpiece. So while it will show you some problems it won't stop you taking a 15mm deep full width cut with a 3mm cutter fed at 1000mm/min. Or setting up the part with the datum in the wrong place so it cuts in a different position, stay tuned for an example of that .



This is a video that I did for something else that shows the simulation in action. First half was the way Bob was going about it working his way down and then a parallel path to do the top. Second half is how I tend to work with an adaptive and then suitable finish paths which was a lot faster and also spreads the wear over more of the flutes rather than just blunting the end.

<a href="https://www.youtube.com/watch?v=w3K6smZ5MWo" target="_blank">http://www.youtube.com/watch?v=w3K6smZ5MWo</a>

[john mills]

those   cad  and graphics  look really helpful  years ago when i started programming cnc, it was all g codes only figures i worked out with a calculator and writtenout with a pencil and typed .
the machining centre had tool changing so it was all automated .you could run though in dry run and see if it was looking ok but there were traps in feed
the machine travelled in a straight line but in rapid could go 45 deg then straight to the end point so crashes could be missed. so basically you had to watch
and be ready to try and stop if it was wrong usually you would be too late.  in years of programming i din't make many mistakes.
John

[Jasonb]

It is still G-code but I don't actually have to write it, just click a button and it comes out in seconds. Just as well as I'm half way through the flywheel and that is about 480,000 lines of code.

[redhouseluv]

Thanks Jason for the detailed explanation, I literally had no clue as to how it works. The simulation mode is clearly key to the processs, so how long did it take to program cylinder 'casting'

Yes I understand, the instructions you give in the software are translated into G-Code which in are sent to the device, much like Arduino uses a simple user interface to control devices.

[Jasonb]

Probably about 10mins as I had to fiddle about a bit to stop the scallop running the tool into the flanges. I have my commonly used cutters in a Libruary so can just click on one and it will have the feeds and speeds I tend to use already entered which saves a bit of time. Actual cutting was about 1hr each side.