What's new
What's new

how to go about machining this job on cnc mill

cuttergrinder

Hot Rolled
Joined
Mar 16, 2007
Location
Salem,Ohio
We have this job at work that we have done before. Its actually the outside link plates for of a very large roller chain. They are about 18" long and 6" wide and 2 1/2" thick. They have a bore in each end and a full radius around the ends. In the past we have just drilled , bored and machined the sides on a horizontal boring mill and then we machined the radius using an endmill and a powered rotary table on a manual vertical mill. Think very very slow.

Now we just purchased a Mazak vtc16 and want to do as much as feasible on this machine. This is the first cnc mill that we have. My plan is do the holes first and then clamp through the bores to profile the outside. This is a no brainer on the cnc but jobs have no holes in them now. Would it be faster to drill the holes on the boring mills and bore them there or machine the bores out on the cnc with a small profiling mill? The bores are about 3". Also if we were to bore these on the Mazak, what type of boring head or bar would be best for the Mazak? We don't have either at this time but we want to buy something but would rather buy the best one for the job the first time.
 
How accurate does the hole spacing need to be? I'm thinking not that critical. If so, bore them out on your manual maybe leaving them 0.05 undersize, then interpolate or bore on the Mazak and then do your profiling bolting them to a fixture. This will save both time and wear on your CNC. As for what boring bar to use, well, I could tell you what we used in 1978, but there has to be something newer now.....
 
2 questions:
1. did you buy rectangular plate thats easy to do a first op on?
2. can you have some construction holes past whats on the print in the final part?

I have done similar items by setting up, blasting some holes for clamp bolts, then coming back in one op complete once I could clamp it..... but you have to have customer approval.
 
The plates are rectangular shaped now. They were supplied by the customer. We cant put in any extra holes except maybe where the corners are going to be removed when we cut the large radius on the ends.
 
What alloy is the plate?
What is the hole diameter tolerance?
How much wider is the supplied plate than the finished link - does that dimension need to be finished, or could you clamp it on those edges?
Does the customer require a machined finish on the outside radius or would another method of cutting be allowed?
 
We have this job at work that we have done before. Its actually the outside link plates for of a very large roller chain. They are about 18" long and 6" wide and 2 1/2" thick. They have a bore in each end and a full radius around the ends. In the past we have just drilled , bored and machined the sides on a horizontal boring mill and then we machined the radius using an endmill and a powered rotary table on a manual vertical mill. Think very very slow.

Now we just purchased a Mazak vtc16 and want to do as much as feasible on this machine. This is the first cnc mill that we have. My plan is do the holes first and then clamp through the bores to profile the outside. This is a no brainer on the cnc but jobs have no holes in them now. Would it be faster to drill the holes on the boring mills and bore them there or machine the bores out on the cnc with a small profiling mill? The bores are about 3". Also if we were to bore these on the Mazak, what type of boring head or bar would be best for the Mazak? We don't have either at this time but we want to buy something but would rather buy the best one for the job the first time.
.
.
machine top
machine profile and holes
flip part and machine chucking stock or the 3/16" held in vise jaws
.
i often used cnc with 4 vises in alignment to hold longer parts. since there is
6 to 8" between vises sometimes part is supported on long parallels that sit
on many vises
 
vises in a row

picture of vises in a row for longer parts
.
obviously you would not need the stops on each vise
 

Attachments

  • MazakVises.jpg
    MazakVises.jpg
    55.8 KB · Views: 258
Could you have the profile and bores flame cut or plasma cut,then throw burn out part in fixture clamping through rough flame cut bores on cnc , machine profile, then hold in soft jaws in boring mill and bore holes ( soft jaws could consist of two six inch vises with profile cut into jaws)???? You could then machine profile in cnc while boring mill was doing the bores.
 
Could you have the profile and bores flame cut or plasma cut,then throw burn out part in fixture clamping through rough flame cut bores on cnc , machine profile, then hold in soft jaws in boring mill and bore holes ( soft jaws could consist of two six inch vises with profile cut into jaws)???? You could then machine profile in cnc while boring mill was doing the bores.
Both of these processes harden the part edges.
 
flat sides?
stock thickness ok for finished parts?
If so to both those, then 2 vises close together to hold one part with big steel soft jaws to hold flat sides and possibly even slight lip over top to ensure no part lift. Then drill and profile both ends in one op and sit back in chair with feet up while it runs.
 
The plates were burned rectangular from 4140 and then heat treated to 27Bhn. So we cant flame cut the rounded end now without messing with the heat treat. I think the rounded ends would have been fine just burned to size if they would of done it before they did the heat treat. Why the customer didn't do this is beyond me. The sides of the plate only have 1/16" of stock left.
 
If you are going to stick to slugging out the holes on the manual, I would switch out to annular cutters to punch them. They make quick clean work for this kind of thing.
 
Why cant you just stick a couple vises on. Using tipped tool m/c side edgeds down to finished size +1m/m reload in vises gripping the side faces do the complete profile.If its acceptable do the bores as a circular pocket all thats leaves is the end holes
 
Maybe I'm missing something, but this seem very simplistic to me.

Clamp rough stock in vise and drill then bore holes

move part to fixture with a locating boss for the holes

machine profile

chamfer

flip to chamfer backside.
 
27 BHN is only 21 Rc so it sounds like they are annealed to get rid of the HAZ after flame cutting and are dead soft. In that state you can cut them with just about any tools that will cut steel. I'd do it like Rstewart describes. If you can get permission to cut the radius slightly large first with a pattern torch that would speed things up but then you have to get under the hard edge of the cut by conventional milling before you finish with climb milling.
 
Mainly what I was wandering is if it would be faster to drill and bore these on the horizontal boring mill or machine out the holes on the cnc. We have done a little drilling and 3d surfacing on this mill but but so far we haven't done any pocketing. The only experience with pocketing on a cnc mill is with my Hurco kmb1 That I have here at home but I know for sure the boring mill would be faster than my hurco. The Mazak has much more power but I really don't know what to expect as far as roughing out these holes with it.
 
Mainly what I was wandering is if it would be faster to drill and bore these on the horizontal boring mill or machine out the holes on the cnc. We have done a little drilling and 3d surfacing on this mill but but so far we haven't done any pocketing. The only experience with pocketing on a cnc mill is with my Hurco kmb1 That I have here at home but I know for sure the boring mill would be faster than my hurco. The Mazak has much more power but I really don't know what to expect as far as roughing out these holes with it.

Those would give your mazak a pretty good break in with a 2-3” shoulder mill with 2 1/2” engaged. Ramping & dropping a slug with a ¾ or 1” endmill will beat drilling, but maybe not annular cutting (pretty expensive annular cutter though).

Just thinking methods & advantages / cost I’d do 3 at a time against a keyed knee for any drilling & boring a 3” hole with a boring mill (3 pass bore for your tolerance @ 63 finish). Spade drill are pretty cheap vs annular & I assume the mill scale is still on the bar. There is no good rotary table solution for the ends unless it’s powered.

Likely the parts were cross cut with a track type bug-o and not a table torch. Going the latter & flame or plasma cutting the holes & ends on a table setup would be a serious up-charge (but not as much as ANY machining on ANY machine tool would be).

Good luck,
Matt
 
I think I'm just going to drill the holes on the horizontal with a 2 3/4" twist drill and bores the holes there. Then put the part on the cnc clamping through the bores and profile the outside with a 2" square cutting facemill. How heavy of a cut do you think the Mazak will take per pass. There is not going to be much stock on the sides but rounding the ends where the plates are now square is going to load the cutter up pretty good. I have to wait until our driver comes in for the facemill. Right now we only have 5 er32 collet holders for this mill.
 








 
Back
Top