Valve Cup Assembly

[petertha]

I'm making my prototype head & valve cups. The plan was turn the cup OD 0.0005" under the matching 10mm hole in head & Loctite in place. I used a 4-flute centering end mill to obtain depth & sharp landing. BTW the hole enters at 22-deg angle into hemi combustion chamber. Unfortunately I’m discovering the hole diameters are not identical. The same valve cup is not slip-fitting as consistently as I’d like. Not sure if it’s the end mill, entering at an angle, my technique or...?

Next I used a 9.5mm end mill pilot followed by 10mm reamer. That achieved very consistent hole diameter & fit results. However the reamer end has ~ 0.035" chamfer so I no longer have the 90-deg ledge. In order to depth match the valve cups relative to the chamber roof & each other, it now has a matching chamfer. Not a big deal but I haven’t heard others reference this aspect. Maybe I’m going about this operation wrong? Any techniques or comments?

Now the valve seat itself. The plans called for what works out to 0.042” diagonal seat, basically full 45-deg chamfer across the cup wall. I’ve followed some of engine builds & that seems on the high side. I've read anywhere from 0.010" to 0.045" but maybe 0.015-0.020” is a reasonable target & also what I measured on commercial RC engine. Sketch shows 0.015” with valve seated +/- across the CC roof. But now I have those odd looking gaps. It’s exaggerated by the scale & section. But I’m more concerned with buildup crap getting lodged up in there. Again any comments or recs on this aspect?

 

[petertha]

Also, I have this Brownells 45-deg chamfering tool coming to dress the valve cup (seat). My understanding is I need to make a center pin that fits the cutter hole & matches the valve stem diameter so it runs true while seat cutting.

But 0.015" seat seems like a teeny, tiny amount. Is this best done lightly by hand? Do you blue the stock first & then check with a magnifier or something? But is it a visual comparison to a 0.015" wire or something or how does one measure? Technique/words of wisdom appreciated!

I just noticed they also sell a goldy colored (surface treated) version of same tool for additional cost. Its too late anyway but was wondering - is the hardness of bronze OK for the cutter edges? Maybe I missed it but guessing its HSS. Can I expect 10 seats without degradation + a whole bunch more 'testers'?

 

[stevehuckss396]

That tool should last you a long time. You will want to cut the seats by hand. The .015 will cut away very fast. Give the tool a twirl to deburr the seat corner. Use a sharpie marker to dye the metal and then cut the seat. The sharpie will help you to see where you are cutting and how much.

 

[gbritnell]

Hi Peter,
Since realizing that valve guides, port pockets and valve seats generally can't be cut concentrically in one setting I have made my own tools much similar to what you show. As Steve said, just give it a light spin with almost the weight of the tool and it will produce the seat you need. I generally try for .020. You can always make it bigger but you can't make it smaller.
gbritnell

View attachment VALVE SEAT CUTTER INSTRUCTIONS.pdf

 

[digiex-chris]

I ran into the same concern about buildup under the valve. Looks like the perfect spot for carbon buildup to me, but maybe it's not a problem. I'm erring on the side of it protruding from the head slightly as opposed to being sunken a little bit.

I like how your cups seat on something and being inserted from the combustion chamber side. I was going to make a fixture to seat them at a specific depth, and then remove the fixture, but I might do it your way. I'm making a very similar head actually, with a hemispherical head (or at least the very top portion of a sphere), and I'm running into trouble accurately locating the valve cup hole. The angle is easy, but how are you dialing in the position of it relative to the sphere while holding it at the angle required? I solved it by coming from the top instead of the underside, but that eliminates the possibility of a lip to butt up against.

Also, how are you cutting the hemisphere? Inside out ball turner?

 

[petertha]

Re the valve depth, I'm more concerned if the low side edge clips the piston on its way up or down although I must admit I haven't sat down to figure out potential interference. The plans show them as quite flush with the CC ceiling. But with my thinner seats it changed the valve elevation down slightly so I’ve had to modify things.

Re the CC hemi shape, I assumed I'd be making a ball turn gizmo. But I tried something easier first & so far looks like it’s working. It’s just a 1/2" HSS tool bit ground with the arc dome profile using a template. Basically it cuts plunge-mode perpendicular to head face. With cutting fluid it yields a nice finish, doesn't rub or squeek. I also dremelled a lip groove to give it some rake & stoned it sharp. I'm less concerned with perfect hemi-ness than yielding identical shapes, therefore equal CR’s.

Re the valve cup drilling operation, I came up with this ‘wedge jig’. So far so good on the prototype. The cad pics don’t quite represent the actual sequence, but I goes something like this:
- Head blank comes off lathe with hemi CC & male lip that protrudes into liner. Then drill/c/bore 5 radial hold down bolt holes
- Head lip fits into matching hole of 22-deg wedge jig & secured with head bolts. I plane off the valve landing to 22-deg bevel angle & datum height.
- Rotate head 180-deg, do other side same.
- Now the bevel face goes down on vice base plate, the jig plate ensures its square in vise jaws.
- I reference measure off the jig hole inside edge & drill the 5mm pilot hole through, then follow with 10mm c/bore for valve cup (that’s now a reamer operation)
- Flip back to topside, locate 5mm hole on bevel deck & make 2 counter-bores to accommodate valve spring & a fitting for rocker perch

A 90-deg turn of head on same wedge jig yields the setup for topside glow plug hole & c/bore. Then different jig for those nasty threaded inlet/exhaust ports.

I keep promising pics. I’ll do that soon once I have a complete head & satisfied procedure will replicate 5+ more. This is my first build so some twists & turns for sure.

 

[digiex-chris]

Good idea! Then you can just pick up the edges of the brown block and dial in the coordinates of the hole. CAD makes a lot of things easy.

 

[petertha]

The brown block is just a cad reference datum representing the mill vise bed or parallels. I actually indicate the valve hole off blue wedge block hole edge once centered. Hopefully this view is clearer. Disregard the little holes in wedge jig, they are head hold down holes exposed from angle cutting the jig plate.

 

[digiex-chris]

how do you indicate off of a slanted hole like the center hole in the wedge block? A DTI sweep would see an oval shape more eliptical than the amount of travel mine has, so I'm guessing just touching off a point, turning the spindle 180 degrees, touching the opposite point, and dividing by two to get the center of those two points? Still, it depends on how far down into the slanted hole the pointer is.

Oh, wait, I think I understand. When it's mounted right side up, you dial in the center hole, which is cylindrical in relation to the DTI pointer. Then flip the fixture upside down, and the hole reference stays in the same spot.

 

[petertha]

1) the assembly is in the vise jaws jig facing up, head on underside resting on bevel deck. So center is first found on lateral distance (orange dashed line) of jig plate which equals attached head

2) with center established, then I edge find on the angled hole, offset distance X to valve center (red arrow) & drill hole

So there is no circular indicating, just edge finding & distances.

 

[digiex-chris]

Makes sense, thanks! This solves the last problem preventing me from getting started on my head.

Back to your original topic, I did some thinking about the problem of inconsistent slip fits with endmills. My experience with endmills seems to match yours. They're far better than twist drills, but still not perfect. I've had quite a bit of good success using d-bit reamers in that situation. You can sharpen it to have a square corner.

That was made out of high speed steel blanks, but I make them out of drill rod/silver steel so that I can easily make them whatever diameter I need. I usually don't buy reamers unless they're a common size that I use often, and instead make d-bit reamers.

Turn and polish to a diameter of the hole you want to cut. Mill slightly less than half the height of the remaining diameter (so more than half is remaining). Harden the drill rod. Then (I usually freehand it), grind the flat you just milled on the periphery of the grinding wheel so that the calipers across the lips you're forming are slightly (0.001") below half the diameter. Because you're using the periphery, the flat won't be flat, but slightly curved. It'll result in the cutting edge having a bit of rake. Then grind some relief on the end, then add some angled relief on the right side of it (flat facing towards you), so that only the one tip is cutting. Usually, with a long hole, I have to bore the start of the hole to the exact size I'm trying to hit in order to start the reamer, but if you keep the reamer very short and hold it stiffly, like in a collet in the mill, you won't have to bore the start of the hole.

http://www.metalwebnews.com/howto/d-bit.html

The most useful thing I've learned by hanging around a clockmaker. You can grind the corner so that the corner of the hole ends up however you want it (rounded, chamfered, etc). They're often used in gunsmithing as chamber reamers.