30cc Inline Twin 4-stroke Engine based on Westbury's Wallaby

Home Model Engine Machinist Forum

Help Support Home Model Engine Machinist Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.


Well-Known Member
HMEM Supporting Member
Dec 29, 2020
Reaction score
Southern California
My next engine build will be a derivative of Edgar Westbury's Wallaby, first designed for a model train, then updated for use in a model hydroplane. The engine is an overhead valve, water cooled, 30cc, inline twin cylinder 4-stroke. My version will use no castings.

I am a huge fan of Edgar Westbury's work as a model engine designer. He was very prolific producing designs optimized for construction by the home machinist with minimal tools, typically a small lathe and a drilling machine. His first engine design was published in the 1920's, a single cylinder 2-stroke for a 13 foot wing span model airplane. He joined Model Engineer magazine in the early 1930's and went on to publish many wonderful engine construction articles as well as several books on machining.

This is a video of a classic Wallaby:

Construction articles for the Wallaby are available from the "Model Engineer" magazine and have been in the public domain for decades. Anyone needing help locating them, feel free to PM me.

The engine has a bore of 1 inch and a stroke of 1-1/8 inches. It has a built in oil pump to provide pressure fed lubrication to the tappets, crank shaft center bush and the connecting rod big ends. I have redesigned the Wallaby to be machined from raw stock, using no castings, and I will be using ball bearings on the crankshaft, camshaft and timing gears.

I use SolidWorks for my computer aided design work and Fusion360 for tool path generation. I first fabricated 3D printed models before committing myself to cutting metal.

The original Wallaby had 5 main castings: the Body Casting, Sump, Cylinder Head, Cylinder Head Plate and Timing Cover.

I have split the Body Casting into three machined parts, the crankcase, rear timing plate and the block. I learned the technique of separating the crankcase and the block from Terry Mayhugh's build of Ron Colona's Offy. When designing a casting, a good engineer will strive to incorporate as many features as possible. This will reduce total part count and reduce cost of a mass production, but results in a very complex part, making it difficult to machine a one off. The Cylinder head has many internal passages that make it a good candidate for a casting, but difficult to machine, so it will likewise be made as two parts to be bonded later with high temperature structural adhesive.

Other design changes include the use of bearing housings for the crankshaft end bearings and the camshaft bearings. This will allow me to fabricate these precision components on the lathe independently from the machining of the crankcase.


My first Goal - Machining the Large components:

  • Sump
  • Crankcase
  • Block
  • Timing Back Plate
  • Crankshaft Main Bearing Housings
  • Dummy Crankshaft
  • Camshaft Bearing Housings
  • Dummy Camshaft

Assembly model of only the large components


Another View


3D Printed Mockup of the engine





I have decided to machine the sump first. It is the second largest part and has many of the same shapes that will need to be machined into the crankcase, so will provide good practice developing the tool paths, tool selection as well as the speeds and feeds. The sump is less critical dimensionally than the crankcase. The crankshaft center bearing is held exclusively in the crankcase and the sump only holds the two bearing housings for the crank case, but will rely on the crankcase for alignment. There will be two locating pins where the sump and the crankcase mate to provide positive, repeatable alignment between the two and the crankshaft bearing housing mating surfaces will be machined from the same setup to provide the best alignment.

Datums for the sump, Top, Right side and Front

Machining Steps

  • Flatten top and Right side of the work piece and insure they are perpendicular
  • Mount the work piece in the vise with Top against the vise face and the Right side down against parallels - machine left side at least .05" over dimension.
  • Mount work piece in vise with the Top against the vise face and the Front down and machine the back side at least .05" over dimension.
  • Mount in the vise with the right side against the vise face and the top down. Machine the bottom square at least .05" over dimension.
  • Take to drill press and drill a 1/2" hole from top, center of sump measured from Right side +.02", from Front +.02", and 1.5" deep (which is more than 1/8" from inside bottom of sump). this hole is the starting point for the end mill to machine the inside.
  • Mount in the vise with the Right side against the vise face and the top up.
  • Machine the inside of the sump. See detail below.
  • Center drill all holes
  • Drill all holes to depth including the two alignment holes. The alignment holes reamed to 1/8" interference fit.
  • Flip part over with Top against parallels, and the Right side against the vise face.
  • Machine minimum clearance for crankcase bolts, leaving the majority of the material to be removed later.
  • Lightly sand the top surface of the sump on a flat surface with 180 grit, then 320 grit and finally 600 grit to create a flat clean surface-don't get carried away, enough to just remove tooling marks.
After these steps, the sump is compete for now and is ready to be attached to the crankcase for the machining of the front and back. 3D modeling programs allow "configurations" of models to be created that are derivative or different than the base part. I use this feature to create modified versions of the model to optimize the machining, creating both models specifically modeled for a specific machining operations as well as special configurations of the stock material. This is nice because as design changes are made to the base part, they are carried forward into the derived parts.

Detail of sump machining operations - A special 3D model is created for the machining of the top of the sump, it has the following modifications:

  • All features are removed from the Front and Back.
  • .020" of material has been added to Front and Right side.
  • Corner fillets removed.
  • Oil drain hole in bottom removed.
A special model is created for the raw stock, it has the following characteristics:

  • square block, .020" over sized on the Front, Back, Left and Right sides.
  • Has a 1/2" hole 1.5" deep in the middle of the sump for the 1/4" end mill that will be used to remove the majority of the material to start in. End mills are great at cutting on their side, but not so good at machining down. By machining from the side of the part, or from a predrilled hole on an interior feature, the pocket machining operation can remove more material, quicker, with less stress on the cutter.

Work piece locked in the vise ready to machine the inside of the sump. The 1/2" hole is used for an entry point for the end mill.


Modified model for machining the inside of the Sump. Compare to sump model above.


Finished inside machining of the sump


Finished bottom machining of the Sump. The sump can now be bolted to the crankcase for further machining.

Lessons learned:

  • I added .020" of stock to the top of the model that was machined off during the first horizontal milling operation. I then switched tools and touched off on the top of the model and my tool path was then .020" too deep. I noticed quickly, but there is an area on the back where the main bearing mount is .020" too deep.
  • When machining the bottom I had problems with the work piece remaining securely clamped in the vise. It was moving during machining. I need to experiment, it may of been due to the fact that the work piece was hollow between the vise jaws, it might have been I just didn't have the vise tight enough, it might have been I did not have a three point clamping points, or I did not have enough of the work piece in the vise.
  • Should have used a smaller step over when using the 1/4" ball end mill on the main bearing housing surfaces.
Things that worked well:

  • I used a two flute 1/4" flat end mill at 8,000 RPM spindle speed, coolant, 15 ipm and .050" depth of cut. I was happy with the rate of material removal and the finish.
  • I did not use a ball end mill on the inside of the sump. My thinking was no one would see the inside, so smooth surfaces were not worth the machining time. However, the surface turned out acceptably well with just with the 1/4" flat end mill.
  • When cutting deeper than the cutter flute length (.75" in my case), I step the material out .010" in the model to prevent the sides of the tool rubbing. This effect can be seen in the deep channels cut in the sump bottom.
Last edited by a moderator:
Hi, you can cast the engine block and other engine parts when you are use the 3D printed pattern in the cast sand and pour direct into, then the pla will burn away. It save a much time.
Also look at what notch you had the vice cross bar in as you can end up with more force going downwards rather than sideways if it is too close to the fixed jaw. I tend to only use my one of these vices where I need the height or jaw opening as I've had stuff move the rest of the time I use a Kurt Copy on the CNC as I find it gives a better grip.

An Adaptive type tool path will give more even wear along the side of the cutter when clearing out the waste in parts like the sump, spiral down say 0.2" each stepdown and then cut using 10-15% of the cutter diameter, set a fine stepdown of of say 0.05" to get the final stepping of the contour.

For something like the bearing housings I would leave metal on them and line bor the two halves when bolted together.

Ahh, I see. that makes sense what you say about the vice cross bar and the direction of force depending what notch it is in. I had not thought of that before. I have limited Z and a Kurt style vise is too tall for my machine.

I will try your suggestion regarding the use of more of the side of the cutter (.2" vs .05") with smaller % of the cutter used each pass. thanks.

I agree with you and will line bore the crankshaft bearing surfaces, I have not done this before so it will be yet another adventure. Mounting the engine perfectly in line with the spindle on the cross slide seems daunting.


I like you casting technique. Casting is something I would like to learn how to do at some point. Right now I still have alot to learn about machining. thanks for the post.
Working on the top crankcase. Here is my plan:
  • Square the stock up on all sides in the lathe.
  • Drill the camshaft hole through the work piece, working from both the front and back, .05" undersized. Use the bottom and right side as the datum.
  • Mount in the mill and using the bottom and the right side as datum, drill and ream the camshaft bearing holder holes from each end.
  • Drill a 1/2" hole approximately in the center of the cylinder as a clearance for the flat end mill to enter.
  • Mount in the vise with the bottom up and the right side against the vise face
  • Machine the bottom using a 1/4" flat end mill. Touch up the crankshaft bearing holder surfaces with a 1/4" ball end mill. Used a .200" step down ( .050" fine step down) with a .050" side cut. 1 hour, 16 minutes total machining time.
  • Machine three flats on the center bearing holder surface, one for a center oil hole and the other two for the middle camshaft bearing mounting screws.
  • Mount in the vise with the top up and the right side against the vise face and machine the top with a 1/4" flat end mill. 28 minutes machining time.
  • Center drill, drill and tap the 6 block mounting holes.

Squaring up the stock in the lathe. I left it over sized, but did not need to "re-square" up the work piece after the camshaft hole was drill and reamed.


Finished bottom machining. You can see small steps .0745" down. the wall sides are .010" thicker so the 1/4" end mill can mill deeper than its .750" flute length. this keeps the mill shaft from rubbing.


Machining the crankcase top surface


I also worked on the block, I brought it to exact dimension on the lathe before machining out the inside.



The engine so far.
The cylinder head is one of the more complex parts due to the fact that there are 7 different surfaces that need machining, five on the outside and two internal, and they must all align as well as possible. The tools that are used include a 1/4" end mill, 1/8" end mill, 1/4" ball end mill, 3/32" ball end mill, spot drill and drills. I did some significant redesign of the head making the following changes:

  • Used larger, yet more cost effective, CM-6 sparkplugs. I had to juggle their position to clear the head mounting screws.
  • I like to use complete bronze valve cages which incorporate the valve guide and the valve seat. the original design has the valves seat directly into the aluminum of the cylinder head.
  • Moved the water jacket holes to give as much clearance to the cylinder head holes, that is maximize the amount of head gasket material between the holes, the edge and the combustion chamber.
  • Rotated the exhaust flanges so the mounting holes do not hit the seam of the top and bottom halves. I don't want the flange mounting screws putting a separating force on the two halves.
  • Adjusted the sparkplug depth and angle to give good access to the combustion chamber, but not interfere with the valve guides.
  • Maximize the water jacket volume without compromising wall thickness.
In order to machine the internal passageways for the air/fuel mixture and the exhaust gases, I decided to fabricate the head from two pieces bonded together.


3D Model of the one half of the cylinder head showing internal passageways

My plan evolved as follows:

  • square up two blocks of aluminum, .25" oversize from front to back and from left to right. Exact dimension top to bottom. Total height of the head is .875, bottom half is .475" thick and the top is .400" thick.
  • Machine internal passages. roughing will be done with a 1/8" end mill entering from the outside of the work piece leaving .010" material. All radii are .1875", so a 1/4" ball end mill will be used for the final finishing passes. Total machining time is 34 minutes per half.
  • install locating pins located in the excess material
  • bead blast the internal passages and the mating surfaces, this increases the surface area for the adhesive.
  • Bond the top and bottom halves of the head using structural adhesive and a sprinkling of 80 grit glass beads. this insures there is a micro space between the halves and the adhesive does not get squeezed out during clamping. Loctite EA9340 is used as the structural adhesive. It has excellent resistance to chemicals including fuels and coolant and is rated to a very high temperature. The alignment pins are used to insure proper alignment, but the three .375" internal passageways can also be used to align the two parts by installing matching dowels. Note: Using the glass beads did not work as they were too big and the two parts just slid around on them like ball bearings and the adhesive would have to be much thicker than I wanted. I ended up just bonding clean parts, but was careful to moderate the clamping force so as to not squeeze out the adhesive.
  • After the adhesive is cured, square the parts up to proper dimension all around.

The two starting work pieces next to a 3D Printed model of the head


Roughing out the internal passageways with 1/8" end mill


Internal passage ways after finish machining with 1/4" ball end mill.


Cured cylinder head work piece, machined to proper size all around.


Machining of the internal water jacket from the top.

The cooling and mounting holes are machined from the bottom as this is the critical mounting surface with the block. I used a 1/4" and 1/8" flat end mills to machine the top. I did not worry about the aesthetics as it will be enclosed and the roughness will not have a material effect of the coolant flow. This is in contrast to the fine finish machining of the air/fuel and exhaust passages that need smooth air flow and thus justified the additional machining time.


Machining the underside - combustion chamber, valve guide holes and water jacket holes. I used a 1/4" roughing end mill, a 1/8" finishing flat end mill and a 3/32 ball end mill for the sparkplug hole.


Finished machining the bottom with the head mounting holes complete.

The mounting holes were spot drilled and drilled through using peck drilling. this is where the drill bit enters about a diameter of the drill bit then retracts and clears the chips, working its way "peaking" through.


I was very happy with the alignment of the internal passages and the valve guides.


Simple jig to provide the proper angle for the machining of the spark plug holes.

A 3D model was created for the machining of these holes using the top edge, closest edge as datums. I am not sure about the proper use of the word "datums" in this context, data is plural for datum, any way I used these edges as my zero points for machining.

Machining is complete. I was happy how the external and internal sparkplug holes met. I did not want to machine the spark plug hole all the way through from the outside as it gets very close to the valve guide, so I machined the internal spark plug hole with the same set up as the valve guides.


Finished Head after bead blasting. I masked the bottom surface, not sure why, probably doesn't matter one way or the other.


Complete head, all holes drilled and tapped.
Great idea bonding the cylinder head together from 2 parts!

Roy Amsbury's V8 used a built up cylinder head as well, though it's silver soldered brass, so it has been done before successfully :)
I am trying a new clamping technique I have seen Terry Mayhugh use to machine flat backed parts that require machining all around the outside boarder- temporarily bonding the work piece to a chunk of MDF. My usual way of machining a part like this is to clamp the work piece to the table with some sacrificial material behind it and clamp beyond the machining boundary. I leave tabs connecting the final piece to the work piece so that the part is held during all machining operations. The problem with this is that these tabs require post machining operations to remove them. I usually cut them off with the band saw, then hand file the last remnants of the rough sawn tab. I am not very good at this and usually file some of the surrounding area or do not get a good blend where the tab was. I figured the Cylinder head cover plate would be a good part to experiment with-it is about a 1/4" thick and 1.75" X 3.25".

I first used the fly cutter to get a nice flat surface on the back side of the part, then used 5 minute epoxy to bond the flat side to a block of MDF. I made the MDF block narrower than the work piece so I could use some shims to space the work piece up from the vise jaws and use them to establish my Z axis zero point. I did not clamp the work piece to the MDF, but instead laid a thin film of epoxy on both the MDF and the work piece, them lightly pressed them together to remove all air. Clamping has a tendency to squeeze out the epoxy and I am not interested in maintaining a dimensionally accurate bond as I will be spacing the work piece off the vise, not the MDF.


Using a fly cutter to prepare a flat rear surface


5 minute epoxy to secure MDF to work piece

I am concerned about the use of coolant while machining as MDF acts like a sponge, soaking up water, swelling and losing all dimensional stability. I fear that using even a light misting may cause problems as the machining operations will be about 45 minutes. On the other hand I don't like running roughing operations where I am removing a far amount of material quickly without coolant; the cutter will load up as the temp of the work piece rises. In the end I rubbed the MDF down with light machine oil and used a small mist of coolant. Let us see what happens.


Work piece clamped in the vise with parallels used to provide proper spacing from the vise

OK, lessons learned. Using both sides of the vise to level a work piece does not work. In my case the clamping jaw is taller than the stationary jaw and the part was machining uneven. I noticed this early so I switched to using parallels under the MDF as is traditionally done. However, due to my caviler bonding process, that is using no clamps, the bottom of the MDF is not representative of the plane of the back of the work piece. Also when I switched to parallels, the work piece was lowered and I did not reset my Z axis zero, so the through holes did not go quite through the part. this can be seen in the last picture below.

Oiling the MDF was not sufficient to prevent water damage, As seen below the outside of the MDF swelled .055".


MDF absorbed moisture and swelled even though only a light mist was used for cooling

Evidence of the swelling of the MDF can been seen in the final part. The final machining operation used a 1/16" flat end mill and the part rose with respect to the cutter by a total of .023" between the commencement of the machining and the end.


.023" trough due to the MDF swelling and the work piece rising during the machining process.

So where do I go from here? I do like the idea of using MDF as a machining substrate as it is much cheaper than using a piece of sacrificial aluminum, for example. The part I attempted the technique with was relatively small and a little moisture on the MDF and the resultant swelling had an outsized impact on the final result. Do I attempt to seal the MDF somehow? Paint? Is it becoming more trouble than the effort saved? I have further experimentation to do.
Quote: "The Cylinder head cover plate will not be permanently attached, but held down by the same studs that secure the the cylinder head to the block. I am working on the head cover plate now. "


This installment will discuss my process for finishing the outside surfaces of the crankcase and the sump. I have found that it is advantages in my workflow to first create a perfectly square work piece to all of the max outside dimensions. In the past I have left extra material on to be machined off at later stages only to mess up because I misremembered what side I left material on, or what the new datum was supposed to be. In hindsight I would have made an exception with the top of the block and left some extra material so I could fly cut the deck after the cylinder sleeves are installed.


Here is the squared up stock roughed out using a fly cutter on the mill.

I have recently been using a new technique, importing a model of the stock into the CAM program creating the tool paths for machining on the CNC router. The program considers the stock to have been machined by a previous machining operations. I am using the free version of Fusion 360 CAM and am pleased with its capabilities (albeit limited).


I create a simple drawing with the necessary dimensions that I machine to using the DRO on the mill.


Once I rough out most of the material on the mill I clamp it to the CNC router bed and machine. I use a 1/2" drill bit and a 1/4" HSS roughing mill at about 1000 RPM on the mill, a 1/4" carbide end mill running at 8000 RPM on the CNC router, then a 1/4" carbide ball end mill to finish the final profile.


I spot drill using the CNC router in the same setup as the main bearing surfaces to insure proper placement. I then take the work piece back to the mill to drill the holes as the CNC router has a very limited Z and does not have room for a tool holder, chuck and drill bit.


Here I am roughing out the bottom of the sump on the mill.



When touching off the part, I do not use just the edges, I will touch off both ends of the part, move the axis to the middle of the two touch off points and then set the DRO to the center dimension of the final part. This way if there is any discrepancy between the drawing and the true dimension of the work piece, the difference is split between the ends and is far less noticeable.


The parts just off the CNC machining the outside profiles. Here I use a .010" step over with the 1/4" ball end mill. It takes about 45 minutes a side. If I reduce the step over, the machining time increases linearly, and if I increase the step over the machined surface is not as nice. I find that .010" step over is a nice compromise. We will see how well the sides clean up and look after bead blasting.


On the sump I machine the two sides and the bottom, each in a different setup
The cylinder block starts with a trued up work piece of 6061-T6. This was done on the lathe, but could have been done with a fly cutter on the mill. After using both, I get more accurate results in the mill, but not quite as nice a finish---probably could if I were more patient.


The first machining operation is from the side to create the internal cavity. I spot drilled the location of the block cover screw holes. In hindsight I would not have done this as I ended up match drilling these holes using the cover plate. My fear was that if I used the spot drilled holes and the cover was slightly out of position, it would interfere with the block to crankcase mounting.

If you look closely at the cavity in the block, you can see a .010" step where the depth of cut exceeded the .75" flute length on my cutter. This technique allows me to cut deeper than the flute length without hitting the shoulder of the cutter.


Next, all of the machining from the top was done in one setup. The large holes for the mounting of the cylinder sleeves were machined at the same time with the same tool to insure concentricity of the hole at the top and bottom of the block. The hole at the bottom is .004" smaller to ease the installation of the sleeve and allow for a cutter to machine only one of the surfaces, top and bottom, at a time. In hindsight I would have left a bit of excess material on the top of the block and used a fly cutter to deck the top after installation of the cylinder sleeves.


A dime for scale, the block is really quite small.

The block cover only required machining from one side so was a relatively easy part to fabricate. I used a roughing pass with a 1/4" flat end mill, a horizontal finishing pass with the same end mill and finally a roughing and finishing pass with a 1/16" flat end mill. this last operation milled the fins and all of the holes.


As mentioned earlier I decided to match drill the holes for the 2-56 cap head screws mounting the block cover to the block. This was done to make sure the cover plate does not interfere with the mate to the crankcase or the cylinder head. I used two .006" shims against a second set of parallels. Since I had previously spot drilled the block and did not want the drill to find these and follow them, I first ran a clearance drill through the hole to create a new spot for the drill to center on the hole before drilling for the tap.


As a rule I don't like match drilling, I believe in building to print. But there are cases where the required precision is too tight to call out on a print and not realistic to call out for fab in my home shop. Other parts where I will match drill include the main bearing housings to the crankcase and sump.


Here I am using the mill to tap the 2-56 holes in the block. A spring loaded tap guide is loaded in the mill chuck. I had to replace the spring in this guide with one much softer as the original provided too great a force for a tiny 2-56 tap. I used the DRO to locate the holes for drilling and tapping.


The block cover in place. I think the block looks really cool, I got the idea for this design from Terry Mayhugh's build of Ron Colona's Offy.


The engine so far.
Time for some Lathe work (or should I say fun ;) )


The bearing holders are fairly straight forward jobs on the lathe. I need to fabricate two main crankshaft bearing holders and two camshaft bearing holders. Here I have the start on one of the Crankshaft main bearing holders and I am test fitting the crankshaft bearing. I used sealed bearing, as opposed to open or shielded bearings. I have used open ball bearings in the past, but used a rifled bronze bushing out board the bearing for an oil seal. At the speeds and temps that this engine will run, the sealed bearings should give good performance and provide a good oil seal. The bearing holder has an oil seal O-ring to seal it to the crankcase as shown below.


The photo above shows the main features of the main bearing holder: a groove for an oil seal O-ring, a .010" relief to clear the ring of the inner race. I first faced the blank, turned the outside diameter, drilled and reamed the through hole to clear the crankshaft. I then used a boring bar to create the features on the inside of the bearing holder. A round tool with the same profile as the O-ring was brought to bear to create the groove.


The holes for the mounting screws in the main bearing holders were drilled on the mill. The inside diameter of the main bearings is .5" and so I used the 1/2 inch dummy crankshaft clamped in the chuck on the mill to align the bearing holder in the mill vise. I then centered the mill DRO at this point and used the bolt circle feature to layout the six mounting holes on each bearing holder. I am using 6-32 socket head cap screws to secure the bearing holders to the crankcase. I first use a .113" drill, the size for the tap, not the clearance hole for a 6-32 screw. I then remove the bearing holder from the mill vise, install it on the crankcase and match drill the holes for the 6-32 threads in the crankcase. Finally, I return the bearing holder to the mill and drill the .113" holes out to .140" in the bearing holder; the clearance hole size for the 6-32 screws.


Now to turn my attention to the camshaft bearing holders.


The camshaft bearing holders were fabricated using the same work flow as the main bearing holders. The primary difference was in the fabrication of the rear camshaft bearing holder. It has an additional feature that routes oil from an oil gallery to the center of the camshaft where oil will travel to the cam lobes.


There is an additional step in the fabrication of the rear camshaft bearing holder, the CNC router was used to create the profile of the flange.


The rear camshaft bearing holder was then mounted in the mill vise and the oil hole was drilled. This hole routes oil to the center of the cam shaft. A hole is drilled down the length of the camshaft to deliver oil to the cam lobes.


The timing cover was machined by the CNC router. Here it is mounted to a block of MDF with 5 minute epoxy. I have had trouble with this technique in the past as the MDF will absorb coolant and swell. Here the technique worked fine as the timing plate is just a 2 dimensional profile and a slight variance in the Z axis will not materially affect the resultant part.


The timing plate is responsible for aligning the bearings for the timing gears as shown in the photo above. There will be a timing cover that holds the mating bearings and encloses the timing gears

I am working on a base for the engine that will also hold the other components required to run: radiator and fan, fuel tank, timing electronics, etc. I also fabricated some engine mounts along with the display pillars and decorative washers.

The engine so far.
Regarding your swelling MDF, you look to be using just standard grade which will be the most likely to swell, Oil will make it swell just like water will. You can also get Moisture resistant which does swell in extreme conditions but should hold up OK for this use and then there is exterior grade which will be even less likely to move. If you only have standard to hand then varnish the exposed faces, epoxy will seal the top so you will only have exposed MDF when the cutter machines any away

I've been using 4 flute ball nose cutters for 3D finishing as you can feed them twice as fast for the same given spindle speed & chip load which halves machining time. You could also probably up the spindle speed too as the effective cutter dia is mostly less than the actual dia of the cutter.

Thanks for the input, I was unaware that there are different grades of MDF, but it makes perfect sense. I just used a piece that was laying around and I am not even sure of its origin. This is good news as I like the technique, I'll google it.

You are correct in that I do use a two flute ball nose cutter and it is a great idea to move to a 4 flute for final finishing. I would be able to make finer passes in less time. I usually leave about .020" of material from the roughing pass, and at really small step overs the cutter hardly removes any material and could run faster. Good idea. Thanks.
When I kicked off the machining of my Wallaby project a month or so ago, I decided to divide the project into four stages. My first was machining the large components and this is now complete with the exception of some cleanup work.

Here is the original CAD design:

And the final result:


Timing Gear side


Flywheel side


The engine looks bigger than it really is, it is only 3 1/8" long!

Next I am going to tackle the power train, not sure if this is proper nomenclature, but I have grouped the project into the 1. major components, 2. the power train, 3. the valve train and 4. the timing train. The power train consists of the crankshaft, middle crankshaft bearing, con rods, pistons, rings and cylinder sleeves. So I will be looking at the crankshaft next. But before I start making chips I need to spend some time working on the 3D CAD model and making a set of prints that reflect the actual dimensions of the parts fabricated. For example, I will measure the distance between the two main crankshaft bearings and match the crankshaft length to this. Another example is the actual center to center distance of the crankshaft and camshaft.

OK, back to the computer.........
Time to start working on the crankshaft. I cut a length of 1 1/4" by 5/8" bar to length and laid out the crankshaft from a 1:1 printout.



Then using a combination of drilling, a compressed air driven cut off wheel and the mill, removed most of the material for turning the first crank pin.

I marked off and drilled the holes on the ends of the work piece with a center drill for turning on centers. Then turned the first crank pin.


I only remove material with the drill and mill as I machine each feature to leave as much strength in the work piece as I can for each operation.

I had a bit of a brain fart and accidently used a dead center in the tail stock when I started turning the first crank pin. I caught my mistake before too long, but may have ruined the dead center. I installed a live center and continued machining.

Then I turned down the second crank pin as I did the first. This was all pretty standard lathe work turning between centers. Since the force of clamping the work piece between centers was straight through the crank pins being turned there was not distortion introduced by this clamping action.

I turned the crankpins to .500" finishing the last thou with emery paper. I am not completely happy with the finish, but they got better as I progressed with the fabrication of the crank. I ground a cutter from a piece of HSS as shown below. The intent, though not necessity executed well, was a broad faced tool at exactly 90 degrees to its length, with a radius on each side and a notch in the middle to reduce the amount of the tool cutting the work piece. I have generous reliefs on the face and sides.


When the crank pins were finished to proper dimension measured with a micrometer, I made some precision spacers to fit between the crank webs. They may not look precision, but I was very careful to make these a good fit, not too tight and not too loose, milling first then running them on emery paper on my surface plate (my band saw table). I made a crank once where these were an interference fit and they actually flexed the crank so that when they were removed the crank sprang back. I bonded them in place with JB weld. Not sure if this was the best choice, the JB weld got soft when the work piece got hot from machining, but it seemed to work out OK.


Here is the setup in the lathe preparing to turn the center main bearing journal.


Here is the center journal for now. I left it .010" over sized because I will finish it to final dimension in a setup where I turn all main journals at the same time to insure concentricity.


To determine the actual dimension between the two main crank bearing inner races, I fully assembled the crankcase, sump and main bearing holders with a dummy shaft with two bearings able to float as shown below.

Then reaching through the cylinder holes in the crankcase I spread the bearing and hot glued them in place. This gave me the actual dimension I needed to turn on the crankshaft shoulders that will rest against each of the main bearings. The design dimension was 2.3125" and the actual measurement was 2.331". I split the difference to maintain a centered crankshaft.

This worked exceedingly well as I ended up with a smooth crank with no end play.


The final operation on the lathe brought the three main journals into concentricity. They were all initially turned to between .005" and .010" over final dimension. I painted them with Dykem and used a thin strip of aluminum in the shape of a tool to rub on the journals to give me an indication of how far out I was. I was surprised that the journals were not perfectly concentric as I had been really careful. So I took very light .001" cuts off each journal walking the carriage back and forth in multiple spring passes. Fortunately I had enough material on them to allow me to produce nice concentric journals. I brought the two outside main journals down to about .0005" over, then removing and replacing the part in the lathe on centers test fitting them to the main bearings. I only used emery paper after I removed the part from the lathe to maintain my concentricity.


I am very pleased as to how smooth the crank turns in the engine now. There is no play in any axis and the crank turns under its own weight.

I have a few operations to finish the crankshaft, I need to drill oil holes that will deliver oil from the center main crank bearing to the big end rod bearings, I need to drill holes through the center of the crank pins (the ends will be sealed with plugs as there will be oil in there) to reduce rotating mass, and I need to add the counter balances.


Crank model with counter balances

I have started researching how to calculate the size and mass of the crankshaft counter weights. This is not a performance engine, won't rev very high, and it is impossible to balance an inline twin with both pistons moving in unison anyway. But I want to get as close as I reasonable can. I am not going to wait to weigh the actual pistons and con rods, but can estimate their weight and center of gravity with the CAD program.

Since the pistons do move in unison the engine can be modeled as a single cylinder engine with twice the mass of one of the con rods, pistons, rings and wrist pins. The formula I found is as follows: Weigh the top half of the connecting rod and add it to the weight of the piston, wrist pin and rings. Then take a percentage, say 55%, and add it to the weight of the bottom half of the rod. Place this weight in the CAD model at the center of both connecting rod journals on the crankshaft. Then adjust the weights of the counter weights to balance the entire rotating assembly.

I will let you know how it works out.

Latest posts