[jpcuttergrinder]

I am new to cnc machining and was just wondering how an experienced cnc machinist would hold an aluminum blank to machine the profile of a rocker arm? The rocker will be 1" thick when it is done. I thought about using a blank that is 1 1/4" thick and holding 1/4" of it in a vise and then milling off the 1/4" on the back after the profile is done. The rocker will have two holes it also. One is 1" and the other is 1/4". I thought about doing the holes first and then make a jig with two pins to come up through the holes to hold it for profiling. The 1" pin would be tapped to accept a bolt for clamping the rocker down.

How would you guys hold this for machining?

[tom bryant]

Hi. jp,
I have built several different style roller rockers for myself over my years of racing. I would be happy to assist you in setting up and machining them.
Your thought about holding them with down with pins and bosses is right on. Make a fixturing plate with a dowel pin going thru the hole where the roller pin goes and then make another tapped pin where the roller brg. or shaft will go. A simple thick washer and grade 8 socket head capp screw will hold them in place for profiling. The selection of material is EXTREMELY important so as to not have the rocker fail from fatigue and stress. Also oiling of the rocker roller and trunion is critical to life support for your engine. If you have furthur questions contact me at: [EMAIL="[email protected]"]
Regards,
TOM

[jpcuttergrinder]

Thanks for the reply. I am thinking of using a material called fortal aluminum. It is supposed to be light as aluminum but it is strong as mild steel. They sell a lot of small pieces on ebay.

[NC Cams]

It is more important that the rocker arm be RIGID than light in the overall scheme of things. "Strond as steel" is but a small criteria for material selection for a rocker. Toughness, fatigue life, notch sensitivity and hot strength are but a few of the other things that you may want to consider.

Although the Jesel aluminum stuff is still perhaps THE predominant rocker of choice in the pro racing circuits (NASCAR, NHRA, etc), billet steel has started to make some serious inroads.

T&D, EPD and several other suppliers (at the behest of the NASCAR crowd) are doing quite a bit in this area and the results are impressive.

Even though the steel is marginally heavier, it is MUCH more rigid - much less of a diving board affect when you get to high RPM. It is also WAY stronger at the same weight and more durable overall.

Considering the fact that NASCAR engines are running at 9300+ RPM for hours on end for HUGE purses, I'd contend that the use of steel for rocker arms is not of fool's wisdom.

[Geof]

Thanks for the reply. I am thinking of using a material called fortal aluminum. It is supposed to be light as aluminum but it is strong as mild steel. They sell a lot of small pieces on ebay.

I looked up Fortal aluminum and I think at least one claim made for it is a bit extreme. Here is a quote;

That and other benefits of the Fortal® aluminum .........also says..... vice president-manufacturing, "There's no expansion of the material from heat like there is with other alloys, and Fortal holds up just as well as P-20 and other types of steel.#quot;

Maybe research the material a bit deeper, it may or may not be suitable but the claim above is not really beleivable.

[Willbird]

Rather than mill the 1/4" off, what I did where I could, and you often can, is mill the profile as you described...then do all other machining in that op, then use a woodruff stype 1/16" wide slitting saw to slice the part off the 1/4" block.....you can often make a profile subroutine and use it to rough, finish, and for the saw too(I wrote the profile for a cutter dia of 0 and used actual cutter dia as the diameter comp...adding .01" for the rough tool for the profile) . I had a 1/2" endmill holder that I cut the nose shorter on so I could saw off thicker parts(cut it back until the setscrew was only in 1/4" from the end) , the woodruff saws I used were 1/2" shank and 1.5" dia HSS...I used them on 4140ht, 8620, M4 and M42, A2, O1, S7 as well as aluminum and plastic so thay will cut most anything if the proper SFM is used, with about .001" per TOOTH feed. The resulting parts were parallal within .001"

[Tornado220M]

I looked up Fortal aluminum and I think at least one claim made for it is a bit extreme. Here is a quote;

That and other benefits of the Fortal® aluminum .........also says..... vice president-manufacturing, "There's no expansion of the material from heat like there is with other alloys, and Fortal holds up just as well as P-20 and other types of steel.#quot;

Maybe research the material a bit deeper, it may or may not be suitable but the claim above is not really beleivable.

Seriously chap you are doubting science ! lol Fortel is just a trade name for 7075 which is a chromium, titanium aluminium, very strong, low density etc etc.... I can't believe you spelt believable incorrectly ..... totally unbelievable lol

https://en.wikipedia.org/wiki/7075_aluminium_alloy

[Tornado220M]

Rather than mill the 1/4" off, what I did where I could, and you often can, is mill the profile as you described...then do all other machining in that op, then use a woodruff stype 1/16" wide slitting saw to slice the part off the 1/4" block.....you can often make a profile subroutine and use it to rough, finish, and for the saw too(I wrote the profile for a cutter dia of 0 and used actual cutter dia as the diameter comp...adding .01" for the rough tool for the profile) . I had a 1/2" endmill holder that I cut the nose shorter on so I could saw off thicker parts(cut it back until the setscrew was only in 1/4" from the end) , the woodruff saws I used were 1/2" shank and 1.5" dia HSS...I used them on 4140ht, 8620, M4 and M42, A2, O1, S7 as well as aluminum and plastic so thay will cut most anything if the proper SFM is used, with about .001" per TOOTH feed. The resulting parts were parallal within .001"

I do it in a similar fashion, I use a Kurt vice for each pair of rockers, one I fit with some special jaws to hold the 2mm at the bottom of my billet the other has soft jaws fitted machined to the opposite ie the shape you are going to cut in op1 but mirrored I then cut everything I can in op1 transfer to the second vice and cut op2 ... that way at the end of op2 you can also machine all your chamfers etc. and every time you open the vice a finished part pop out .... well it does for me but I use a 4th axis to rotate the whole fixture including vices to drill countersink then tap the adjuster part.