What's new
What's new

V8 Blocks and heads on 4020 mill?

snowshooze

Hot Rolled
Joined
Sep 15, 2010
Location
Anchorage, Alaska, USA
Hi Guys;
Lots of people asking for engine work now our local shop rolled up.
Is anybody doing this stuff in their VMC?
I have Fadal 40-20 ( x 28" ) with VH-65 indexer..
Thinking of building the biggest trunion table I can get in there... like 16" x 36" x 1"+ thick 7075....
It would be nice to see some setups.
Oh, and is there a catch-all reference for specifications that the automotive guys reference for things like bore sizes and allowed head material removal?
I have done a few flat heads on the Haas and Dah-lih to good success, but I make my Customers figure out how much I can remove.
Thanks Guys!
Mark
 
Blocks reference off the mains so you use a bar, not a table.

I would buy automotive machining equipment if that's what I wanted to do. A CNC mill is not going to win it for whatever walks in the door automotive engine machining.

I would buy quality new CNC stuff designed for what you want to do. Real hard to make a living doing the newer engines with old machines.

Anchorage is a pretty big city. There's really no engine machine shops there?
 
There is a reason there are dedicated cnc machines (centroid most notable).

Also, there is an astounding amount of engine knowledge you'd have to learn in order to ever make a name in that niche market.

Sent from my SM-G955U using Tapatalk
 
Blocks reference off the mains so you use a bar, not a table.
?

So production block machining is done off of the mains locating on a bar?
Agree that this would be best but the mains are cut off of something and one datum for the entire process would seem to simplify things.

Auto remake machines are generally sort of flimsy but setups are easier than a VMC and the machine made for the purpose.
Boring and honing a BB Chevy on a trunion table is going to need a whole lot of Z stroke not to mention trying to line bore the mains.

How much stock you can take off of a head varies by casting and valve train layout so no fixed rule of thumb.
Newer engines are more sensitive to remaching than older ones and made to tolerances that would be very hard to duplicate on a VMC.
In the old days removing .060 from a head a common practice to reduce head cc volume. Now that might have a valve/piston clear problem.

For sure it can be done.
I would think a 40x20 maybe a bit on the small side for blocks but maybe okay for heads.
On a head or deck I like to see at least a 12 inch diameter cutter so you have to get this off both ends of the part.
Also in big use the spindle head is tilted just a tad so that the trailing edge of the cutter does not touch. This on a VMC means making the machine into a single use thingee.
And there is the wave as one goes from full part contact to almost none as you pass the chamber or bore.
Making a part that "runs" and one that will go 200,000 miles not the same so one can get away with a lot on a rebuild.
I've done more than a few Chevy, Pontiac, and Ford heads on a 10x50 B-port clone. Would not try to bore these on this but have bored a few bike/lawnmower types on such.

Overall... heck give it a try if the cost not to big and you can afford to throw it away. One never knows the limits until you try.
I will not say no and I will not say yes so I am of no help at all....:dunce:,:dopeslap: and for sure just another talking head on the net.
Bob
 
I have both a dedicated block , head machining center , rottler and a vmc 4020 with a 4th and extended z. If you wanted to just do automotive engines up to a bb chevy you could do it. Most blocks at the factory are machined from the pan rail on a fixture with shot pins, its just easier to get stuff in the right place using the mains. Your going to have to make some tooling for boring, and as far a tipping the head not really needed in my opinion. Your going to want to use cbn inserts for cast and pcbn for aluminum. Single cutter in a 12 inch balanced fly cutter type tool. And be damn carful on your speed coding as if you add a zero on the end of your s1000 you better run FAST! There is a thread of that happening. Think cannonball!
A 90 degree head will line bore quite nice as long as you can access the bore.
Rottler uses one they build and uses boring bar cutters from their cylinder bars. It can all be built just takes time. Or if you feel flush, the machine from Rottler is north of 100000.00 us and for only about that much more you will be tooled for about any engine up to 50 inch length you could run into. Im going to be rebuilding one this winter , if the control is dead looking at a centroid possibility as they already have some automotive history, and the have probing routines for finding cylinder bore centers and other engine features


Sent from my iPhone using Tapatalk
 
So production block machining is done off of the mains locating on a bar?
Agree that this would be best but the mains are cut off of something and one datum for the entire process would seem to simplify things.

Auto remake machines are generally sort of flimsy but setups are easier than a VMC and the machine made for the purpose.
Boring and honing a BB Chevy on a trunion table is going to need a whole lot of Z stroke not to mention trying to line bore the mains.

How much stock you can take off of a head varies by casting and valve train layout so no fixed rule of thumb.
Newer engines are more sensitive to remaching than older ones and made to tolerances that would be very hard to duplicate on a VMC.
In the old days removing .060 from a head a common practice to reduce head cc volume. Now that might have a valve/piston clear problem.

For sure it can be done.
I would think a 40x20 maybe a bit on the small side for blocks but maybe okay for heads.
On a head or deck I like to see at least a 12 inch diameter cutter so you have to get this off both ends of the part.
Also in big use the spindle head is tilted just a tad so that the trailing edge of the cutter does not touch. This on a VMC means making the machine into a single use thingee.
And there is the wave as one goes from full part contact to almost none as you pass the chamber or bore.
Making a part that "runs" and one that will go 200,000 miles not the same so one can get away with a lot on a rebuild.
I've done more than a few Chevy, Pontiac, and Ford heads on a 10x50 B-port clone. Would not try to bore these on this but have bored a few bike/lawnmower types on such.

Overall... heck give it a try if the cost not to big and you can afford to throw it away. One never knows the limits until you try.
I will not say no and I will not say yes so I am of no help at all....:dunce:,:dopeslap: and for sure just another talking head on the net.
Bob

We've had a few threads on this topic before (I know, I started one of them).

We know blocks were not fixtured off the main line during original machining. The factory made everything line up and fit right, but that doesn't mean that the pan surface actually relates to anything.

I think if you specialize in one kind of engine you can develop a process and fixtures that make a big VMC viable.

I just cannot see it working for whatever comes in the door though.

I still cannot fathom there aren't a half dozen or more engine rebuild shops in Anchorage. Anchorage is a big place. 291,000 people live there. My town of 34,000 has one race engine builder, two brick and mortar engine rebuilders and another half dozen "rural engine builders" with old machines in their barn.
 
i think you will find there is not much time in Reconditioning a engine and setup speed counts for allot, the old way of grinding seats takes time the new way of cutting seats and vacuum testing is only 12 min on a 6 cyl 4 valve head if your setup correct and have good gear.
Still nice to have the grinding gear to touch up a seat...
look into Rottler products, i have not used them but i know i don't like Serdi ( Italian machine ) its not so good.
Sunnen are the people for honing machines.
Rottler Manufacturing | CNC Engine Building Machinery and Equipment
Sunnen | Sunnen - Partnership. Precision. Performance.

the setup off the mains is a Square bar with knocked off edges ( precision ground ) it locates on the edges a round bar won't work.

there are of course other machines as well i would have to talk to my friend who does the work to what they are now.
 
As others have said, automotive machining is a whole nother skill set with different tooling needs. People ask me if I can bore a block on my HBM, I tell them yes but you don't want to pay that much. What grit hone do you use to finish it? What do you do for a fast setup? Line bore it with what? Then their are valves and seats, grinding cranks, etc.
If there is enough demand buy out the machines and hire the old operator, maybe he can fill in on conventional work. From the way auto machine shops are going away around here it will be a war of attrition.

Ed.
 
Yeah, I am aware, and am thinking on the main bearing fixturing aside. But for wedge heads, it's either build a fixture, or easier, a universal trunion table in conjunction with the positioner.
I am thinking the capabilities of the machine are beyond the specialized equipment in many ways.
Thanks!
Mark
 
Having some background, enough to be dangerous, I do realize.
The dedicated machines, I am thinking are possibly designed for those that are less the Machinist, and more the production Automotive shops as our equipment takes yers to become proficient due to their universal capabilities.
Thanks!
Mark
 
Thanks Bob;
The Fadal has 2500 hours and excellent.
Holds tenths very well.
I did a Kia head last night with a 4" 5 insert shell, 12mm round positive plain sharp inserts.
3 passes to get the width, abour 8 inches, .003 DOC 7 IPM around 2500 RPM...
Came out all aces. Yes, you could see the 3 passes, however, you could not feel them, fingernail or other.
I really believe it stands up. And that was on the old Dah-Lih Rigid head mill. Of course, the only tram runnout would be that it is a knee mill, but the thing is massive.
I have never been scared of holding tenths before, do it daily...
And I am pretty sure you do too.
I am thinking it is more stigma than fact. ( But this is why I am asking you guys! )
Thanks!
Mark
 
Yeah, even more people than that now.
But, Eagle River, one small shop buried in work, or Palmer.
Fortunately, I have 28" Z on my rig, so it is easier, plus I have a jib crane for loading right over it.
I am accostumed to Boring Mill work where I would load and machine Chassis for loaders...
Parts weighed tons. Crane loaded tooling too.

The wole thing is I see a project... well-head, Blowout preventer... motor block as being only different in shape.
I am looking for the holes in that theory, and appreciate every single bit of wisdom you guys offer!
The biggest concern I have I guess is fixturing on a reletively small table, and still providing the rigidity to avoid harmonics and chatter.

Align boring is another matter, although I do have a home-spun rig, I also have a right angle head.
Problem is too much for the vmc due to having to move the cutter in the bar to pick up the journals.
Can be done in one pass with the home-spun rig, but I am thinking to just take a rain-check on that job.
Thanks!!
Mark
 
Yeah Ed, got most of that.
My intention is to taks only jobs I am sure of, and talking with guys like you is the first thing in identifying the pit-falls.
Deck keads, bore jugs, a lot is a snap. Wedge heads, one step up.
Blocks, a couple steps.
Thing is, a jig-work shop is not what guys like us have, so hiring an expirenced hand would bring great knowlege, but he probably would be a ways from doing setups at our level, or any of the horsing about we have to do.
Thanks!
Mark
 
Thanks Bob;
The Fadal has 2500 hours and excellent.
Holds tenths very well.
I did a Kia head last night with a 4" 5 insert shell, 12mm round positive plain sharp inserts.
3 passes to get the width, abour 8 inches, .003 DOC 7 IPM around 2500 RPM...
Came out all aces. Yes, you could see the 3 passes, however, you could not feel them, fingernail or other.
I really believe it stands up. And that was on the old Dah-Lih Rigid head mill. Of course, the only tram runnout would be that it is a knee mill, but the thing is massive.
I have never been scared of holding tenths before, do it daily...
And I am pretty sure you do too.
I am thinking it is more stigma than fact. ( But this is why I am asking you guys! )
Thanks!
Mark

I think right there you've shown you're a machinist and what you don't know about engine rebuilding.

Modern heads, decks and bores require specific surface finishes. Flat is critical, but you actually need a little rough for MLS gaskets. Honing is another area where a non-CNC hone cannot do the finishes modern engines require.
 
Very good points.
Specs I can hit. RMS, flatness...
However, the first concerns I see up front is positioning and avoiding harmonic chatter, things of that nature.
I have 28" Z axis, which won't hurt anything. A boring mill it aint.
The hone is CNC when it is hanging in the Fadal. Chrome rings us a differnet crosshatch then Iron. Do I want to ruin my Fadal with grindings?
Nooo. I do filter to 5 microns, but the idea is repulsive.
But there is that old mill over in the corner..
Plenty stuff like that.
No, it ain't easy.
Yeah, land-mines everywhere.
And I have to thank you for making sure I am aware!
Mark
 
I've done a few on my leadwell MCV550. Its an old machine but works good. Bored and counterbored out a few inline 6's done a few v6's. I have wedges that are the degree of the head and go off the pan rail. A little shimming required to get it true but a cylinder's a cylinder. Indicate it in and it will be good to go imho. It always takes me longer than the dedicated auto machine shop but sometimes they're booked months so I get a little work from them. I've even honed on the VMC but it was difficult. No coolant and lots of oil and filters to catch the oil and grindings. Rather hone it on the floor with oil and use my sunnen 815 with the proper stones, much easier to hit diameter and finish that way. I don't do valve work, just deck blocks, heads, bore, cut for studs, few other things. I explain I'm not a race shop but will get it back to running condition if its fixable.
 
I've done a few on my leadwell MCV550. Its an old machine but works good. Bored and counterbored out a few inline 6's done a few v6's. I have wedges that are the degree of the head and go off the pan rail. A little shimming required to get it true but a cylinder's a cylinder. Indicate it in and it will be good to go imho. It always takes me longer than the dedicated auto machine shop but sometimes they're booked months so I get a little work from them. I've even honed on the VMC but it was difficult. No coolant and lots of oil and filters to catch the oil and grindings. Rather hone it on the floor with oil and use my sunnen 815 with the proper stones, much easier to hit diameter and finish that way. I don't do valve work, just deck blocks, heads, bore, cut for studs, few other things. I explain I'm not a race shop but will get it back to running condition if its fixable.

Yeah, looks like a fair amount of easy stuff to pick up if I take it.
No need to try to go crazy with it.
Thanks!
Mark
 
A VMC cannot do what a CNC cylinder hone does.

Go watch a CNC hone working.

First time I did I was amazed.
 








 
Back
Top