GDB4 - Inline 4 Cylinder, 4 stroke IC engine by George Britnell

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
GDB4 - Inline 4 Cylinder, 4 stroke IC engine by George Britnell

I am kicking off another engine build and as my last was a twin, I thought I might move up to a 4 cylinder. George Britnell has always been a hero of mine and has made available plans for an inline 4 cylinder that meets my criteria as a next build. George is a true craftsman and does incredible work. I am very fortunate that he has taken the time to create plans of his masterpieces so that I can continue to build my skills as a hobby machinist and fabricate one of his engines. I know I will not be able to meet his exacting standard, but I hope to end my quest with a running engine.

First, several photos of George's engine to get motivated.


This will be the smallest engine I have ever built, so I will be challenged by the smaller scale. My last engine used 6-32 screws to secure the oil pan to the crank case, this one uses 0-80. Yipes.

I looked over the plans of the crankcase, as good a place to start as any, and established that the most critical aspects of the design is the relationship between the crankshaft and the camshaft. They need to be perfectly co-linear and the proper distance apart since a set of timing gears reside between them. I have decided to let the camshaft be my first major datum.

Working from CAD models helps me visualize the engine and allows me to develop my machining strategy.

Lets make some chips!

My plan is to square up a block of aluminum for the crankcase oversize by .050" on all sides, then drill and reamed the .3125 hole for the camshaft.
First I squared up the block of aluminum on the mill, then moved to the lathe to drill the camshaft hole. I did not have a drill long enough, so I drilled most of the way through with a standard drill bit, but then finished the job with a custom D-bit made from .3125 drill rod. I had to cut a .0625 groove down the side of the D-bit as air would get trapped inside and I couldn't push the bit in to cut. If you look closely at the D-bit you can see the groove.

Once I punched all the way through with the D-bit, I followed up with a reamer. Fortunately my reamer was long enough to make it all the way through.

Below is a picture of the crankcase with a .3125 drill rod installed in place of the camshaft. This is now the my master datum and I will create other features from this.

I squared up the bottom and the left side of the crank case to the camshaft on the mill. These two sides are now square to the camshaft and can be used a datum planes for future milling operations. Next I plan to machine the crankshaft referenced to the camshaft.

I took a strip of aluminum with the same cross section as the crankshaft main bearing caps and using a 1/4" ball end mill, mill a slot down the middle .125" deep. My intention here is to create a matching groove down the bottom of the crank case where the crankshaft will be centered. This will allow me to place the crankshaft exactly where I want it with respect to the camshaft.

Then I cut a matching groove down the crankcase perfectly positioned with respect to the cam shaft.

Finally I clamp the long bearing cap strip to the crankshaft using a 1/4" drill rod to align it to the crankcase and drill the crankshaft bearing cap mounting holes.

Once I screw the bearing cap strip down I will ream the crankshaft hole to size.
Hope this all makes sense.
Crankcase Bottom Machining

I tap the bearing cap screw holes in the crankcase using a taper tap first, then a bottoming tap. The bottoming tap only buys me three more threads so I am not sure this extra step is worth it. The bearing caps will be held on by 2-56 screws.

Then I screw the bearing cap strip in place.

Then I drill and ream the final hole through the crankcase and bearing caps. I reamed the inside diameter of the bearing caps to .374" as my Bronze bearings will have an OD of .375".

Below is a picture of the bearing cap strip removed.

And finally I complete the machining from the bottom side of the crankcase.

You can see the pocket for the camshaft and I am pointing to one of the oil pan screw holes, these will be tapped 0-80. I also spot drilled the oil holes that will feed the main bearings.
In hindsight I should have left the bearing cap strip in place and machined the bearing caps at the same time that I machined the internal cavities.

Next I will machine out the cylinder water jacket from the top side. I machine the outside features very last as I like to have the outside square and flat as long as I can so I have something easy to clamp on to.
It's great to see another one in the works! Should you have any questions at all please don't hesitate to contact me.
Cylinder Block Top Machining

Now to turn my attention to machining the top of the cylinder block. But before I do I want to machine the tappet cavity in the side. this is indicated below.

Since I am still working with a large chunk of aluminum, I need to machine down a bit to get to the pocket.

Below you can see that there looks like there is a pocket inside a pocket. I do this because my 1/4" end mill only has a 3/4" length cutting flute and the tappet pocket is deeper than this. I don't want to rub the edge of the end mill on the upper pocket. Also you can see that the upper pocket has only a roughing mill pass, while the deeper, actual tappet pocket also has a finishing milling operation.

I make a 3D model of cylinder block with only the water jacket area around the cylinders features present. Note the extra material at the top that needs to be machined off because I originally squared off an over sized block for the work piece. In the picture below this extra material is semi transparent and indicated by an arrow. Also you can see a ledge that has been incorporated to the model. This machining operation requires a reach deeper than my .75" flute length end mill, so at .7" I step out a tad to prevent the side of the end mill from rubbing as i mill further down. I know, you are thinking why don't I just buy a longer fluted end mill. I could, but I am altering the design to accommodate what is in my tool drawer.



Then I likewise create a model for the holes on the top of the cylinder block.


My little CNC router does not have much Zed clearance, so I can't drill, so I essentially use a small end mill to spot drill, then go to the Mill to drill, ream and tap the holes as applicable.


And below is the final result of the cylinder block top and bottom machining.

Great work!
Thanks George, that means a lot. :)

Machining the Front of the Cylinder Block and the Oil Pan

My next area of focus is the front of the cylinder block, but I want to machine the front of the oil pan at the same time to get a nice blend between them.

So, to the oil pan. First the inside. I square up a block of aluminum to the total outside dimensions on the mill, load it into the CNC router vise and let-r rip. I run three programs, one to rough out most of the aluminum, one to finish the flat bottom surfaces, and one to finish the curved surfaces that ride against the main bearing caps. Finally I use a 1/16" end mill to drill the .070" clearance holes for the 0-80 hardware to secure the oil pan to the cylinder block. There is a 5 degree draft on the sides of the oil pan, but I did not run a finishing pass on these as they will be inside and not seen. You can see the roughing steps in the long inside wall of the oil pan.


I need access to the complete outside during the machining operations for the bottom and sides, so traditional clamping does not lend itself well. Instead I clamp an old 2X4 into the vise and using a wood router bit, flatten the top and cut a small ledge near one edge (see red arrow below). By pushing the oil pan down flat against the smooth routed surface and up against the little ledge, I have squared the part with the X, Y and Z axis of the CNC router. I use 5 minute epoxy to secure the work piece to the block and wait an hour before machining. I run three programs, a roughing pass to remove most of the material, a horizontal pass to give me a nice finish on the top and the flats where the screws mount. Finally I use a ball end mill on the rounded corners and the sides, which have the 5 degree draft. I use a .004" step-over on the sides, but 5 degrees is really too steep to get a nice finish on my machine. It might have been better if I had finished the two sides separately from the bottom, but it would have meant two more set ups and the alignment of the side to the bottom is problematic. This way I have nice corners, but the sides will require more finishing work by hand.


For machining the front of the engine, I need to secure the oil pan to the cylinder block, so I start by tapping the 0-80 screw holes in the cylinder block.

In my quest to find small hardware I tried some screws I had in a glasses repair kit, but the threads were wrong. I lucked out and my hardware store stocks #0, #1, #2, #3, #4 and #5 hardware. But just like Henry Ford's Model T, they come in any color you want, as long as its black. Fine for now.


In the photo below I have highlighted a few features on the front of the engine that need special attention, particularly the fillets, or absence of them. Where the timing gear case rises from the front of the engine, there is a 1/16" radius fillet all the around, except where the water pump mounts. Also, inside the timing gear case there are no fillets to clear the gears.


Below are a couple of examples of models to get the CAM program to give me the tool paths that I want. For example, the top photo cuts the clearance for the water pump.



Above is a photo on the machine as the final finishing passes are run with the 1/8" ball end mill.

The photos below are right off the machine.



I will machine the back of the cylinder block and oil pan in the same manner. It is starting to look like an engine.
Great documentation!
Dodged a Bullet Today

I made an error this week machining the Block Top Plate and it really gave me pause. The part needs to be .227" tall and I started with 1/4" thick stock that ended up .242" after I had squared it up and fly cut the top and bottom. When I programmed the tool paths in Fusion360 I miscalculated the amount of raw stock to be removed from the top (.242" - .227") and I machined too much material off and ruined it. The top plate is relatively simple and was easy to remake, but what if I had made this mistake on the cylinder block? I have been working on the cylinder block up to this point and have innumerable hours into it. The thought really upset me. I got lucky and dodged a bullet on this one. I need to remain ever diligent and check everything multiple times (I thought I did).

The Block Top Plate seals the water jacket in the cylinder block.

The good part is sitting on top of the block and the bad part is in my hand,

I also machined the back of the cylinder block and the oil pan in the same manner as the front as seen in my last post.


Next up is machining the sides of the cylinder block.

I made the Top Plate wider than it needs to be because I am going to secure it to the cylinder block and then machine the sides of the bock with it in place.

But now I am going to kick back, enjoy the sunset and meditate on my luck.
Intake Manifold
Today I am going to be working on the Intake manifold, it can be seen below in green and indicated by the arrow. I am going to be attempting Terry's Epoxy Encapsulation Technique (TEET) as the part is machined from two sides and work holding would be very tricky otherwise.
I design the part, then the encapsulation fixture. I go to the mill, square up a block of aluminum, then measure it and put the exact dimension back in my model. There is a runner that needs to be drilled all the way through to create the internal fuel/air passage from the carburetor to the cylinder head. Then aluminum plugs are turned on the lathe for a snug fit and pushed into position just the right depth.


The drawing below has all the dimensions I need to fabricate the initial fixture/work piece including the through hole and the aluminum end plugs for the lengthwise fuel/air passage. Note that I have also drilled two 5/16" end mill entry holes into the work piece. My little CNC router complains when I drive an end mill straight down into the work piece, but if I provide the entry hole then only side mill, I can run at higher speeds without stressing the setup.

The tool paths are created and simulated. I use an adaptive clearing strategy to remove most of the material, a ramp strategy to mill the vertical sides, a horizontal strategy to mill the flat horizontal surfaces; these all use a 1/4" end mill. A 1/8" ball end mill is then used to create all of the internal and external fillets.

Below is the work piece after machining the top.

I then use 5 minute epoxy to encapsulate the intake manifold. The amount of epoxy used was great enough that the exothermic rection of the mixed epoxy cured very rapidly and I did not need to wait long to move on to machining the back. I then repeat the tool path generation and machining of the back side. When I touch off on the back side I am careful to use the same datum points as I did for the top as it is very important that the two machining operations meet as accurately as possible so the features are not noticeably offset.

Below is the back side of the work piece after machining. I am pleased with the alignment of the top and bottom machining operations.

I then heated the part for 1 hour at 275 degrees as Terry did. The 5 minute epoxy I used did not decompose, but just got soft. I was able to remove the intake manifold from the fixture, but as the part cooled the epoxy just got rock hard again. I think I just post cured it. I had to reheat and then work quickly with a rag to remove as much of the softened epoxy as I could. I used "Quick Set" epoxy from Ace Hardware instead of the Devcon 5 minute epoxy Terry used. Most of the epoxy reside was removed as I did my final filing and hand finishing of the part, and the sand blaster got the last of it. I did not want to use a higher temperature as I used Loctite 638 to secure the end plugs, which is a high strength, high temp adhesive, but it too will get soft at higher temperatures.



All for now, thanks.


  • 1637605930006.png
    407.6 KB · Views: 77
Machining the lobes of the Camshaft

The machining of the Camshaft lobes is done using a 4th Axis on the CNC. The Camshaft is cut from 5/16" drill rod and uses the OD as the bearing surfaces. There are bearing surfaces at each end and between each cylinder. The cylinders alternate between having the intake lobe closer to the front and the exhaust lobe closer to the front. This is done to simplify the design of the intake and exhaust manifolds. I am going to machine a single cylinder's pair of lobes in one machine set up, thus will have four setups on the CNC.

A 3D CAD model of the camshaft sections is created for both the intake manifold lobe in front and the exhaust lobe in front. A feature is added as shown below and highlighted with the red arrow to create a coordinate system the CAM software as a reference for the tool paths. There are four separate tool paths. I could have gotten away with two tool paths then adjusted the starting rotation of the work piece before each machining operation, but I opted to make the setups as easy as possible even if it required a little more work before hand.

Then each of the four tool paths are simulated.

All four machining operations will be done as close to the collet chuck as possible to minimize the stick out, so a method needs to be used that allows the work piece to be extended and reoriented before each machine run. The work piece is prepared as shown below with a flat machined at the far end.

A simple carpenter's level is modified with an aluminum guide that rides in the flat, then is secured to the work piece with rubber bands.

This provides a simple and accurate way to return the rotation of the work piece to a known zero point. I am able to easily discern a tenth of a degree of rotation when jogging the A axis.

The stick out is simply measured with a caliper to the face of the collet.

Once the CNC is touched off on all axis, it is ready to run.

The cut is done in three passes, two roughing with a .025" step down and .025" step over. The finishing pass uses a .0075" step over. Mist coolant is used.


The work piece is stepped out of the collet before each of the four machining operations.


And the machining of the Camshaft lobes is complete. The remaining machining and finishing work for the Camshaft will be performed on the lathe.
Beautiful work! The camshaft came out great!