PDA

View Full Version : Fly cutting cast iron



michael3fingers
05-16-2009, 07:42 AM
HI everyone.

I am new to machining and I have just started flycutting some cylinder heads for my mini.

I was using a face mill but I have just started using my fly cutter and some 3/8 tool steel.

I ground it with a bit of an angle on the face.

The end result is better but its still pretty average and I could certainly not charge for that kind of job.

I have a RF 45 Clone that I ran on the next speed up from slowest.
I fed the work into the cutter really slow and took only a very light cut.

Any Pointers?

http://i92.photobucket.com/albums/l13/mickstar_2006/Picture314.jpghttp://i92.photobucket.com/albums/l13/mickstar_2006/Picture313.jpg

thanks everyone

websterz
05-16-2009, 12:24 PM
HI everyone.

I am new to machining and I have just started flycutting some cylinder heads for my mini.

I was using a face mill but I have just started using my fly cutter and some 3/8 tool steel.

I ground it with a bit of an angle on the face.

The end result is better but its still pretty average and I could certainly not charge for that kind of job.

I have a RF 45 Clone that I ran on the next speed up from slowest.
I fed the work into the cutter really slow and took only a very light cut.

Any Pointers?

http://i92.photobucket.com/albums/l13/mickstar_2006/Picture314.jpghttp://i92.photobucket.com/albums/l13/mickstar_2006/Picture313.jpg

thanks everyone

Looks like your machine may be slightly out of tram. All the visible tooling marks go the same direction. I bet the cutter is taking a bit more on one edge than it is on the other.

Once you resolve that issue if you still don't have the surface you desire you may try lapping the part on a hard flat surface with some 600 grit wet/dry paper.
I lap cast iron dry, seems to work better for me.

Also some close-up pics of your cutter would be helpful. Fly cutters can be finicky to grind.

Scishopguy
05-16-2009, 06:02 PM
If you grind a small radius on the tool bit/bits in the fly cutter you will get a little better finish. Try not to take too light a cut, like one or two thousandths, as a little heavier cut will give a better finish. That is about all I can add. ;)

Carld
05-16-2009, 06:03 PM
The problem was speed and feed. You should have run 800-1000 rpm and taken light cuts with a moderate feed. You won't get a good finish with a slow rpm flycutting anything. Each and every pass is a seperate cut that shows on the surface of the work.

Tram/sweep the head in as close as you can posibly get it, hold the head on the table as strongly without warping it as posible and use about 1000 rpm and .010-.020" DOC. On the last pass use .002-.005" and a steady moderate feed. If your feeding by hand you can see and feel the feed rate you want after some experience.

.RC.
05-16-2009, 07:38 PM
Looks like your machine may be slightly out of tram.

Production machines run like that deliberately to speed up production..
The amount of concaveness on the part is insignificant...

websterz
05-16-2009, 09:28 PM
Production machines run like that deliberately to speed up production..
The amount of concaveness on the part is insignificant...

Well if he is new to machining, as he says he is, he certainly isn't cranking them out by the gross. His machine is out of tram regardless.

I have been a production machinist for over a decade and I never set my machine out of tram to speed things up. :confused:

Greg Menke
05-16-2009, 10:50 PM
Thats a big radius for 1k rpm.. I'd set the rpm to something close to that suggested for cast iron sfm (refer to feeds & speeds in Machinery's Handbook- probably something between 40-100 rpm), and put a radius on the cutter edge (and correct the tram). That much radius out from the spindle may be unavoidably limber, particularly on a light mill- so go easy on the depth of cut & feed.

Greg

.RC.
05-16-2009, 11:08 PM
I have been a production machinist for over a decade and I never set my machine out of tram to speed things up. :confused:

http://www.practicalmachinist.com/vb/showthread.php/tram-mill-best-surface-163990.html

knedvecki
05-17-2009, 12:00 AM
We just about always "Set our heads a little out of Tram" in production work so that the heel / trailing side of the cutter would not drag to make a better finish, say about .002 on a 6 inch diameter sweep. And I would use a brazed cemented carbide lathe tool bit in my flycutter to minimize tool wear.

Tim Clarke
05-17-2009, 12:45 AM
Looks like something is moving around to me. When I had a RF-30, I used to surface exhaust manifolds with some sucess. the trick was to get everything as solid as possible. If I was to surface heads, I'd be putting the head on parallels, and checking for a rocking situation. A couple pieces of threaded rod down thru either the sparkplug holes, or valve guides are the classic way to secure cyl heads, when possible.

That head looks like a 950cc BMC head as used on a Austin I had back in the dark ages........ Best of luck,

TC

michael3fingers
05-17-2009, 08:05 AM
well...

my first problem was that I had the tool bit 90 deg out.

I spent about half an hour tramming the mill and now I am just getting the crosshatch pattern so I think I will leave it. I did it over and over with the dial indicator just sliding on the bed but it always seemed a bit out once I tightened it up.

I had more luck just bumping it with some wood and then doing a cut and repeating until I got it close. My bed must be a bit out or something.

I am trying to keep the cut as light as possible but its hard with the crappy indicator on the quill. I have ordered a digital scale so once that's here 002 - 003 thou cut will be a bit easier.

I have found a better way of mounting it to the table so now ridgidity is not much of a problem. And I will be able to mill right off the end.

I just have to refine my tool grinding skills and it should better as time goes by

Its a mini 1098 head . 12g202 :D

pics
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture352.jpg
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture342.jpg

Mcgyver
05-17-2009, 01:03 PM
I would doubt that mill will go slow enough for a tool steel (which i assume means HSS) cutter.

RPM = cutting speed * 4 / dia. For everything, drilling, milling, lathe etc. Cutting speed for hss and cast iron is say 80 feet per minute. As a guess maybe the dia is 4 or 5 inches? means the mill should be going no more than 50-80 rpm. When your mill won't go so slow, a you can use carbide which will work at higher speeds.

The problem is going to one or more of..... incorrect tool geometry (do some searches, somewhere here I've posted pics and diagrams for fly cutters ), incorrect speed and maybe not enough rigidity in either machine and/or fly cutter set up.

Sorry to sound like a nanny on this, but you really should crack a text book and study the basics - how cutting speed works and how to calculate, how metal cuts and where and what the corresponding rake and clearance angles should be etc. Almost all metal cutting comes down to these basics and machining and troubleshooting are night and day when you understand them.....things'll get a lot easier :)

Spin Doctor
05-17-2009, 06:01 PM
Is it just me or is one of the combustion chambers a different shape :confused: In a production invironment the surfacing of heads is usually done with shell mills that utilize a wiping insert. You really only want such an insert cutting on one side

davidh
05-17-2009, 06:19 PM
just out of curiosity, does the surface need to be glass smooth or just flat ?

and, mini ? as in cooper ?

aboard_epsilon
05-17-2009, 07:05 PM
you are supposed to be able to start off the head and end off the head ..even a Bridgeport with a 42 inch table will struggle ,even with a mini head ..........looking at that circle at the end of the cut ..that's were your table travel ended.

I've been told it's not advised to do what you're doing, if you haven't the table travel .

the only way you could make some attempt at it ..would be to machine to the middle of the head ..stop ..

then start at the other end ..and machine into the middle again ..but i would be thinking oh no to that as well.

so you need a very good unworn Bridgeport with a 48 inch table .

all the best.markj

Carld
05-17-2009, 07:29 PM
First, your not going to get a smooth finish running below 500 rpm on that head.

Second, you should be using the knee to feed the table up, not the quill to feed down. The knee is considerably more accurate than moving the quill.

lazlo
05-17-2009, 08:24 PM
We just about always "Set our heads a little out of Tram" in production work so that the heel / trailing side of the cutter would not drag to make a better finish, say about .002 on a 6 inch diameter sweep.

There are two counteracting effects here: for general accuracy, you want the mill trammed as close to dead nuts square as possible (as John Oder and others pointed out in the PM thread). But when you use a large diameter flycutter or facemill, the cutting forces will lift the leading edge up and twist the quill, which drags the heel of the cutter, and leaves a strong trailing edge swirl.

The amount of twist depends on the size/rigidity of the machine, the amount of runout and dynamic stiffness of the quill bearings.

So some production shops will tram the leading edge slightly low -- i.e., around a tenth per diameter of cutter. That will allow the leading edge to cut, and the trailing edge will stay off the workpiece. It leaves a shallow scallop, but for a production shop that's doing a lot of slab milling, it saves a lot of wear on the cutter.

Tramming the leading edge low is probably not a great idea for HSM'ers or mills used for a variety of jobs (other than flycutting), since it's intentionally adding inaccuracy to your setup for a single purpose. But then again, you never get the tram exactly 0.0, so I usually try to err on the side of the front edge being a little low. At that point, you're tweaking the torque on the head bolts anyway...

By the way, Carl's advice about using the knee and minimizing the quill stickout is right on -- there's a lot more twist and flex with the quill extended.

Carld
05-17-2009, 08:55 PM
The main reason I suggest traming the head as near "0" as posible is the load on the bearings by the flycutter. When the cutter is cutting on the leading side the cutter is pushed up and when it on the trailing side it cleans the cut. When done that way the surface is as flat and smooth as it will get. You will never get rid of movement in the quill to housing and the bearing movement so you have to compensate for it.

michael3fingers
05-17-2009, 11:39 PM
First, your not going to get a smooth finish running below 500 rpm on that head.

Second, you should be using the knee to feed the table up, not the quill to feed down. The knee is considerably more accurate than moving the quill.


I dont have any other means to feed my tool and work together. I have a dovetail rf45 clone.

So I have to run +500 rpm with a single point hss cutter at a 4 inch sweep ?

michael3fingers
05-17-2009, 11:43 PM
you are supposed to be able to start off the head and end off the head ..even a Bridgeport with a 42 inch table will struggle ,even with a mini head ..........looking at that circle at the end of the cut ..that's were your table travel ended.

I've been told it's not advised to do what you're doing, if you haven't the table travel .

the only way you could make some attempt at it ..would be to machine to the middle of the head ..stop ..

then start at the other end ..and machine into the middle again ..but i would be thinking oh no to that as well.

so you need a very good unworn Bridgeport with a 48 inch table .

all the best.markj

I have more than adequate travel. I just stopped where I did because I had not perfected my clamping technique. Its all fixed now.

I have seen with my own eyes mirror finish on a similar head with a lesser machine
http://home.exetel.com.au/zoomini/zoomini/Heads/IMGP0933.JPG

michael3fingers
05-17-2009, 11:45 PM
just out of curiosity, does the surface need to be glass smooth or just flat ?

and, mini ? as in cooper ?


yes mini as in cooper...

from what I have been told just smooth enough so that your finger nail slides across it easily

michael3fingers
05-17-2009, 11:51 PM
I would doubt that mill will go slow enough for a tool steel (which i assume means HSS) cutter.

RPM = cutting speed * 4 / dia. For everything, drilling, milling, lathe etc. Cutting speed for hss and cast iron is say 80 feet per minute. As a guess maybe the dia is 4 or 5 inches? means the mill should be going no more than 50-80 rpm. When your mill won't go so slow, a you can use carbide which will work at higher speeds.

The problem is going to one or more of..... incorrect tool geometry (do some searches, somewhere here I've posted pics and diagrams for fly cutters ), incorrect speed and maybe not enough rigidity in either machine and/or fly cutter set up.

Sorry to sound like a nanny on this, but you really should crack a text book and study the basics - how cutting speed works and how to calculate, how metal cuts and where and what the corresponding rake and clearance angles should be etc. Almost all metal cutting comes down to these basics and machining and troubleshooting are night and day when you understand them.....things'll get a lot easier :)


hi grandma....glad you finally found the internet;)

rigidity is a problem as its a 4 inch sweep. I am using 3/8 steel as a cutter but I have another head here that I am going to mill out to .5 inch soo that should help

I also have a proper face mill here that I will use for getting the surface up to scratch before I make a light single pass with the fly cutter to get a nice finish on it.

I will look for your cutter shapes right now....

could you recomend some reading?
thank you

michael3fingers
05-17-2009, 11:54 PM
Is it just me or is one of the combustion chambers a different shape :confused: In a production invironment the surfacing of heads is usually done with shell mills that utilize a wiping insert. You really only want such an insert cutting on one side


yeah its all different. The heads full of cracks so its just a mule so to speak.

Mcgyver
05-18-2009, 09:30 AM
hi grandma....glad you finally found the internet

yeah, machinist's tough love. I almost didn't write that bit ....didn't want to be another grump telling a newb to figure it out himself; but it really is sincere advise....you or anyone will get so much more out of it and come up the curve much more quickly with that little bit of theory on how metal is cut. Why i did bother was i was impressed with what you were doing - seemed fairly industrious fly cutting those heads so i thought this is no ordinal newb.

As for recommendations, Moltrect's two volume "Machine Shop Practice" is excellent and well worth having - might seem a little heavy for a newb but you won't outgrow it. Pretty much any grade 11/12 machine shop or college text book would be good, shouldn't be too much money either if you can find an old one - the advantage of these is they're written for the inexperience so are easy to follow. Another classic is the Amateur's workshop by Ian Bradley and to move far away from the textbook format but still full of good info are Latuards 3 "machinist bedside readers".

Online for free, there's the US army machining coarse. Dry and slow but the bases are covered :)

lakeside53
05-18-2009, 10:57 AM
What's the url for the Army course?

lazlo
05-18-2009, 01:05 PM
U.S. Army "Fundamentals of Machine Tools"

http://www.metalwebnews.com/machine-tools/fmt.html

Carld
05-18-2009, 02:48 PM
michael3fingers, that last photo looks like a good finish. What was the spindle speed, DOC and feed rate?

michael3fingers
05-18-2009, 11:56 PM
michael3fingers, that last photo looks like a good finish. What was the spindle speed, DOC and feed rate?

it was done by my old mentor on a manual machine. It was done at around 110rpm and cranked very slowly by hand. The cut depth was only about 3 tho...

Thanks for your help everyone. No offense taken, were all here for the same reason..

Carld
05-19-2009, 09:46 AM
Yep, it would have to been VERY slow feed to get that finish at 110 rpm but the .003" DOC helped.

After having used flycutters as a full time machinist for over 20 years now I can assure you the finish will be better at a higher rpm. Here is my collection of flycutters and some ground cutters. The smallest is 3/4" dia. and the largest is about 3" dia. and the various cutters are for specific jobs and finishes. If you experiment with high rpm, feeds and DOC you may be surprised at the excelent results you can get. Of course in a factory or job shop you have to find the best and fastest way to do a job. For a smaller mill such as yours you may have to balance the flycutter to reduce vibration and you always have to be able to machine past the ends of the work. You can't stop the cutter and reverse the direction while the cutter is still on the work surface. I have on occasion had to move the cutter off the side of the work when I didn't have enough travel on the table. While that's not the best way it was the only way to cut the entire surface and get an acceptable finish.

http://i82.photobucket.com/albums/j276/yeathatshim/flycutters-2.jpg

michael3fingers
05-24-2009, 07:38 AM
I got a chance to do some more machining today.

I made a small correction to the tram of my machine and now its spot on.

I have been playing with cutter shapes and have found one that gives a usable finish.

My cutter was running at 97rpm and my DOC was 2 tho and my feed rate was about a foot in 20mins.

I think it needed another run but heres some photos.. It will be perfect eventually.

Ignore the gouges etc in the head..

http://i92.photobucket.com/albums/l13/mickstar_2006/Picture399.jpg
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture392.jpg
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture410.jpg
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture408.jpg

michael3fingers
05-24-2009, 07:40 AM
http://i92.photobucket.com/albums/l13/mickstar_2006/Picture398.jpg

lazlo
05-24-2009, 09:54 AM
It looks great! :)

websterz
05-24-2009, 11:42 AM
Just enough texture for the gasket to get a good bite. I think you're done! :D

Alistair Hosie
05-24-2009, 04:59 PM
I agree with it being out of tram but the tool also badly needs proper sharpenning from the scoring.Alistair

michael3fingers
05-24-2009, 08:22 PM
thanks al

I will look for some sharpening info any that you know of?

also I would thing that the tram is pretty spot on? is that not the case?

thanks for your responses

Carld
05-24-2009, 09:13 PM
The crosshatch pattern tells me your head is tramed right but your spindle rpm is still to slow. There is no reason to run it that slow and have to take 20 minutes or more to make a pass on the head. The finish could be much nicer by just speeding up to 500rpm and going to 1000rpm would be better. Set the cutter diameter to clear the sides of the head by a 1/2", make a full pass to clear the tool on each end.

It looks like you have a radius on the cutter, is that right? You could stone the cutting edge to get a finer finish on the head. It don't have to have a texture to "grip the gasket", that's been proved to not be needed.

tattoomike68
05-24-2009, 09:19 PM
Cast Iron can be harder than you think, ditch the HSS and use carbide. A cheap C2 brased tool bit will do a fine job.

Carld
05-24-2009, 09:24 PM
I would suggest the same thing, especially if he ever decides to go to a good working rpm for the spindle. As long as he stays under 100rpm and slow feed on soft metal he can get by with HSS or maybe Cobalt HSS. Flycutters hammer the hell out of HSS as I found out long ago.

aboard_epsilon
05-24-2009, 09:29 PM
1000 rpm ..hss.... cast iron ..no way

the hss cutter would die

he's sweeping something like 6 inches there

i think he's done as well as can be expected and picked the right speed .

Not sure about the profile of his cutter ..but it's done the job and that's what matters .

Cutters are sharpened the same as a lathe tool ..all you got to remember is its upside down and at an angle ..so imagine it the right way up and level ..and you got it .

all the best.markj

michael3fingers
05-24-2009, 10:41 PM
its a 4 inch sweep.

It does not hammer at all with low RPM and a fine DOC it just makes a nice "cutting sound".

I will speed it up a little but I wont go to 1000rpm. The thought of doing so go against all the formulas I have come across.

I will look at the cutter shape.

boslab
05-25-2009, 04:20 AM
I watched a vid on tv recently that showed a rebuilding of a landrover block, it was fly cut but the guy said id was some kind of diamond[?]tooling, i cant imagine a diamond taking it but he could have been refering to a brand of ceramic or somthing, anyway the rpm was about 200ish by looking but more importantly he had a substantial circular guard over the flycutter, and it wasent the lightweight cutters ive seen so far, it was a heavy trpanning cutter with a 1 1/2" square bar as the arm and a single cutter.
anyway apart from that well done, the head looks good fine tuning is all thats needed, i have got the same finish with a 50" table cincinatti but the flycutter was not up to the job, i'm fiddling with a sandvick 14" inserted tooth facemill at the moment, looks promising
once again well done, its really nice to so folk having a go
mark

Carld
05-25-2009, 09:16 AM
Aboard, if your refering to my post #38 you didn't read it correctly or completely, go back and see what I posted. It's right above your post last post #39, page 4.

Michael, you did fine and you would never be able to run HSS above maybe 150rpm for the 4 inch span. If you don't mind spending a half an hour to make a pass manualy cranking the table that is ok.

Since you don't seem to be interested in experimenting with anything but HSS you will have to take what you get. Maybe at some point in the future you may decide to try brazed carbide cutters with different tip shapes and then you will discover the versitility of the flycutter. Actually you get less hammering at a higher rpm than lower rpms. Also, a flat leading cutting edge will hammer like hell and if you grind a leading angle there will be very little hammering. A radius on the cutter gives a fine finish but doesn't like much DOC. We did work with flycutters that most people would not think posible because it was the fastest way and you didn't have to have special cutters ground up, you could grind the cutter yourself and single point the work.

aboard_epsilon
05-25-2009, 09:31 AM
i was refering to post 36 ..


The finish could be much nicer by just speeding up to 500rpm and going to 1000rpm would be better. Set the cutter diameter to clear the sides of the head by a 1/2", make a full pass to clear the tool on each end.


then you changed your mind in 38

all the best.markj

michael3fingers
05-25-2009, 09:44 AM
OK thanks for your help everyone. I will look at different cutters. I am not against it I was just trying to do the best with what I have. I don't mind the fact that it takes so long. I am in the process of making an auto feed for it .

michael3fingers
05-25-2009, 09:48 AM
http://cgi.ebay.com.au/12MM-1-2-5PCE-INDEXABLE-CARBIDE-TIP-LATHE-TOOL-SET_W0QQitemZ380125083405QQcmdZViewItemQQptZAU_BnI _Woodworking_Metalworking?hash=item588138770d&_trksid=p3286.c0.m14&_trkparms=66%3A2|65%3A1|39%3A1|240%3A1318|301%3A0| 293%3A1|294%3A50#ebayphotohosting

something like this guys?

dockrat
05-25-2009, 12:18 PM
Michael, your link will not work as posted but by searching Ebay with the item number, I found it. I would not recommend that set. I have one of those that came with my lathe and it is just junk. The inserts can move around in the tool mount. I think what the guys here are recommending for your fly cutter is something like this: Search Ebay for item 360118047315

AEP
05-25-2009, 06:07 PM
I'd say the finish is a little too smooth. A rougher cut holds the head gasket in place better. The rule of thumb is....Drag penny across the milled surface. You should leave some of the copper penny on the machined surface.

Just my opinion,
Andy

aboard_epsilon
05-25-2009, 06:43 PM
I'd say the finish is a little too smooth. A rougher cut holds the head gasket in place better. The rule of thumb is....Drag penny across the milled surface. You should leave some of the copper penny on the machined surface.

Just my opinion,
Andy

is that old advice ..for old types of gasket

isnt it different for the new mls gaskets ..ive heard it has to glass smooth for them.

all the best.markj

Carld
05-25-2009, 10:04 PM
Aboard, in #36 I thought he was using carbide, I didn't change my mind.

I agree, as I said in a early post, the surface doesn't have to be rough to hold the gasket. As Aboard said, that is old school and no longer used. In fact it was never needed, just thought it was needed.

michael3fingers
05-26-2009, 01:25 AM
I found something local and it looks like a good idea. Its the right diameter and its quite long so that would help with the balance as the tool needs to be about 75mm out from centre.

270394076858

looks good ?

michael3fingers
05-26-2009, 09:13 AM
those were boring bars


I just found these ones. Would these different angles all be of some use for what I am doing?


ebay no. 270397389299

aboard_epsilon
05-26-2009, 10:40 AM
those were boring bars


I just found these ones. Would these different angles all be of some use for what I am doing?


ebay no. 270397389299

there maybe one in that whole set that you could use ..to explain the rest

there are right hand tools ..left hand tools ..and strait on ..in that set..

i cant work out without having one in my hand ..and looking at the flycutter ..and observing the rotational direction .

really what you want, if you are going to be doing a lot of heads (expensive when not busted like this one) is one of these that is over four inches wide

http://cgi.ebay.co.uk/Milling-Cutter-Indexable-Milling-Lathe_W0QQitemZ230344600098QQcmdZViewItemQQptZUK_H ome_Garden_PowerTools_SM?hash=item35a19baa22&_trksid=p3286.c0.m14&_trkparms=66%3A2%7C65%3A7%7C39%3A1%7C240%3A1318%7C 301%3A1%7C293%3A1%7C294%3A50

All the best.markj

MrSleepy
05-26-2009, 03:56 PM
Heres a video of someone skimming a head on a bridgy with a homemade skimming tool...there's also a video of the tool construction if you look in his collection ..
http://www.youtube.com/watch?v=cR-vQ2sCBrE&feature=channel
Rob

Peter.
05-26-2009, 07:05 PM
I'd say the finish is a little too smooth. A rougher cut holds the head gasket in place better. The rule of thumb is....Drag penny across the milled surface. You should leave some of the copper penny on the machined surface.

Just my opinion,
Andy

For modern steel layered gaskets you don't want that kind of roughness. It's usual to have cylinder heads and barrels lapped very flat for those leaving a fine surface finish.