"Mould Making......My way"

[Red River Rick]

I just finished cutting the cavities on a couple of new moulds for one of our members and thought some of you may be interested in seeing how I machine mine.

Last week I finished making 80 mould blanks so that I'd have blank blocks in stock and ready to go. When I make my blocks, I do so making them six up at at a time rather than individual blocks, saves lots of time this way.

Now all I have to do is finish off with the sprue plate holes, adjustable base plate and some engraving.

The picture showing the close up of the finished cavity is right out of the machine, no polishing and no hand work.

I do not cut my cavities using cherri cutters, as of yet, but have opted to machine them via "3-D Surfacing" with the CAD/CAM system that I'm running. All my moulds are CNC machined.


RRR

[felix]

RRR, please put Sundog and me on your first mold(s), other than for yourself! ... felix

[kodiak1]

now felix there is a slim posibility there are two of them that I asked for back in December!!!!!!!!!!

LOL Ken.

[Lloyd Smale]

so are you going into bussiness and going to offer custom molds in various configurations. What i see looks great and i could see a full time job for you just taking over the lee group buys on the group buy site!!!

[Topper]

Looks like your designing a top pour mold, similar to Hoch.
Is this correct?

[Red River Rick]

Felix:

Your going to have to wait your turn, these are spoken for, but I can most certainly reserve one for you and Sundog.


Ken:

Your very observant, and yes this is one of yours. I will have them out in the mail next week, thanks for being patient.


Lloyd:

I have to learn to walk before I can run, but yes, my intent is to eventually do this type of work on a full-time basis. I'm still perfecting my cherri making, and so far I've had some excellent results. Time will be the factor, and until that time comes, I'm limiting myself to the simple moulds.

As far as group buy mould go, I've been looking at a brand new CNC turning centre (lathe). With this machine, a whole lot more would be possible, I'm saving my pennies, just another $30,000 to go.

Topper:

Yes, this mould is a nose pour design and will have an adjustable base.


RRR

[felix]

Thanks, Rick. ... felix

[Buckshot]

.................How fast is that shaper tool spinning? It all looks neat (as I turn my cranks and stare at my DI's :-)).

...............Buckshot

[Red River Rick]

Buckshot:

I was using a 1/8", four flute solid carbide ball nose endmill for the roughing cycle. Spindle speed was 4500 rpm, feed rate - 18 ipm, depth of cut - 0.040" and the step over was 0.030", leaving approx. 0.005" for the finishing.

Total cycle time for the roughing was about 20 minutes.

The finishing pass was done with a 3/16" ball nose endmill, spindle speed 5500 rpm and the step over was 0.005". Cycle time for the finishing pass was approx. 20 minutes as well. I usually run the finishing pass twice, this helps clean up if there is any "Tool Deflection".

I always machine with coolant, tends to give a better surface finish and besides, carbide endmills don't perform as well if they have to "recut" chips. I also use brandnew endmills for my finishing, they in turn, will be used for roughing on another project or another boolit mould.

RRR

[JIMinPHX]

If you go to a 1/4" 2 flute ball mill & a slower spindle speed for your roughing, you will be able to get that pass done in about a minute. It shouldn’t take any great effort to change the program. Cutter comp should be all you need to adjust. The larger diameter mill will allow you to take a heavier cut. The larger radius of the nose will allow you to use a larger step-over without getting a higher ridge. A two flute mill will give you better chip clearance & is the next best thing to a genuine roughing tool. If you are cutting aluminum, then there is no reason to use carbide. High speed steel will do at least as well at a much lower cost. I concur that flood coolant is definitely your friend in these operations.

[JIMinPHX]

Those are some nice looking blocks that you have there.

Did you intentionally leave the flycut rough so as to form vents? That seems like it might be a nice way to do it if you did.

[no34570]

Wow,they are nice looking moulds
Can you make them in any caliber?,say 44 for a 444 Marlin? and a 44 Mag to start with.
cheers
no34570:drinks:

[Red River Rick]

JIMinPHX:

Yes, I concur, a larger diameter BN end mill will create less scallop when using a larger step over but in this case speed is not the important factor. I am partial to using 4 flute BN end mills for finishing because they do provide a better finish. I can remove twice the amount of material using a four flute BN end-mill when finishing than opposed to a two flute BN end-mill.

I have hundreds of solid carbide end mills in my shop, and probably only have two HSS end-mills. Why anyone would bother using HSS end-mills in a CNC milling center, just doesn’t make any sense. You cannot obtain the accuracy and the speed & feeds with HSS as you can with carbide, that’s why “GE” developed carbide during the 2nd WW. HSS tooling just didn’t “CUT IT”.

Same with aluminum, if you’re working with 6061 or equivalent, HSS will do just fine. More a few grades up to say 7075 T6 or 2024 T6 and see how long your HSS tooling lasts. Carbide will outperform HSS nearly all the time.

Actually speed is not the driving factor for which I have set out to achieve; QUALITY rather than QUANTIY is the driving force. Sure, I can crank my machine up so that I’m machining at 500 ipm and wind the spindle up to 8000 rpm and pump moulds out faster than you can shake a stick at. But, how many of those are you going to be tossing into the garbage?

And besides, when my mill is running, I can run the lathe or do other things.

I’m striving to deliver a top quality product at a reasonable and affordable price. There would be nothing worse than making a bunch of “s*+” and having some customer buy it. I can assure you, you won’t be selling anymore to him, not to mention every other person he talks to as well. And on this board, news travels fast, you may just as well crawl into a hole someplace and hide. And hope the guys don’t find you.

No34570:

I try to stay away from anything smaller than .375. But your needs would be no problem, any diameter you want.


RRR

[JIMinPHX]

No offense there Rick, I was just suggesting that you might want to speed up your roughing pass. I didn’t want to imply that you should shortchange your finishing work in any way. It’s just an old habit of mine to try to get the roughing knocked out quick. I did a lot of production work & I was always building gang tooling & stuff like that to reduce the number of tool changes that I had to make so that I could shave seconds off my cycle times.

I’ve generated many thousands of pounds of aluminum chips myself over the years, so I do have a little experience with that stuff. Mostly I stuck with 6061-T6, but I have done some work with 7075 (expensive) & 2024 (soft with high tensile) before too.

In many applications, high speed can outperform carbide due to the high speed being less brittle & having greater natural lubricity in some materials. Carbide is the obvious choice in hard or abrasive materials, but HS still has it’s place too. It even gives better finishes in some cases where the tool can be held short to maintain rigidity or in a material where the carbide tends to gum up. In some applications, like cutting annealed titanium, HS far outperforms carbide. Of course, once you make a mistake & get the Ti too hot & generate a hard spot, then you need carbide to get things started again. Ti is scary stuff to work with, welding or machining.

Carbide is a wonderful material. It was one of the German’s biggest advantages in the early days of WWII back when it was a Krupp kept secret. It allowed them to produce parts efficiently that we could not. Carbide makes the machining of many difficult materials possible & even practical, but it is not the best answer to every application. Cermets are one step past that. They are even harder & more brittle than the cemented carbides are. When trying to get a good finish in a hardmetal turning operation, I reach for them, but that is the only time that I reach for them.

I didn’t mean to insult the quality of your work in any way. Those are some nice looking blocks that you have there. I was just trying to toss a possibly-useful piece of info your way. Sorry if it seemed otherwise.

Regards,
Jim

[Red River Rick]

Jim, no offense taken, all you’ve said has been taken highly, obviously you are knowledged in the operations of CNC machining, not many of us out there. I’ve been a Journey Man Tool & Die Maker for almost 25 years (one more month to go), and have spent the last 17 years running CNC VMC’s. I run a Bridgeport VMC 1000/22 at work and have my own Haas VMC at home, I sometimes wonder why, could have bought that new F-250 Super Duty diesel with what I spent on the Hass.

With regards to the venting on the blocks, I did attempt to use a face milling cutter in order to obtain some form of venting, but that didn’t work out as well as I had anticipated. Even with a slow spindle speed (150 rpm) and high feed rate (80 ipm) and a shallow depth of cut. I ended up milling some venting on one half of the mould (see pic) using a 3/16” carbide blank sharpened to a triangular needle point. It worked out quite well, I admit it was slow going but the end results will suffice.

Seems to me, after close examination, that a lot of OEM use some sort of “Scribing” method to produce their venting. Perhaps manually or with the use of a “shaper/planer” type of operation.

Like I mentioned, I appreciate your input, and absolutely no offense taken.

Thanks.
Rick

[IcerUSA]

3R's , you could try a conical point split end blank or a single flute half round end mill for your vent lines or maybe a heavy 1/2 " solid round carbide scribe point . Jusy a couple ideas to look at . With aluminum you could get by with HSS I would think also . The cut won't be very deep so most any type pointed cutter should work and you can program it to not vent right on the nose like some moulds I've seen .

Keith

[JIMinPHX]

Thanks Rick, I’m glad to hear that I didn’t tick you off. My intentions are generally good, but my elocution is not always what I intend it to be. I didn’t realize that you had as much experience at this as you do. I wouldn’t want to tell Campbell’s how to make soup.

Haas is always very nice stuff. I’ve used their multi axis indexers & other small accessories. You did not short change yourself by passing up on a nice truck to get a machine like that.

With regards to venting, I haven’t actually made any blocks myself yet, but I’ve been toying around with a few different ideas on how I might best make vents. My first thought was to kick a mill head off at a 45 degree angle & drag the corner of an end mill across the face of the block at a few thousandths depth every 1/4" or so. Tramming the head back straight is kind of a pain in the neck, so I would rather avoid that unless I was going to do a large enough batch of block blanks to make it worth the work. My next idea was to use a flycutter. What you described would seem like the most efficient way to do that, but I thought that I might get better results by plunging the flycutter a few thousandths below flush & then moving over 1/4" & doing it again, & so on, & so on. This would require a fly cutter with a radius that exceeds the length of the blocks being worked on. I have a 14” flycutter somewhere that was mounted on a 40 taper. I may need to dig that up If I’m going to try that trick. I’m not sure how well people would take to curved vents though. They should work fine, but they may look funny to people that are used to seeing straight lines. My last idea, involved scribing, but I thought about doing it by hand. I was thinking of making a jig to control the depth of the scribe’s cut & also hold it straight. I figured that a setup like that with a handful of shims to move it down the block face in even increments might be the quickest, easiest & most universal way to go. I just wasn’t sure about the quality of the vent lines that I would be cutting with a scribe. I don’t really know much about what kind of tool point geometry would work best for a scribe like that. That had me thinking about setting up something more like a router guide if I couldn’t get the finishes that I wanted off the scribe. I’m still kicking ideas around. I’ll let you know if I come up with something that I actually like.

Again…nice job on those blocks

Regards,
Jim

[Red River Rick]

I have a 14” flycutter somewhere that was mounted on a 40 taper. I may need to dig that up If I’m going to try that trick. I’m not sure how well people would take to curved vents though. They should work fine, but they may look funny to people that are used to seeing straight lines.

Jim:

I don't think looks would be an issue here, as long as the venting worked and allowed the boolit to fill properly. The radial venting, using the flycutter, would be most efficient way and probably provide the best results.

Unfortunately, I can't swing the head of my mill off by a few degrees. Who knows, maybe a 5 axis machine would be in order.

Thanks again.
Rick

[JIMinPHX]

If you have a big enough fly cutter, you can just plunge straight down with it & get a half of a scallop. If the fly cutter is wide enough that it only hits the block on one side of it’s arc, this should work with a 90 degree spindle.

[JIMinPHX]

The 14" flycutter that I was talking about holds the tool bits pointed straight down. it's easy to get good tool tip orientation on that one using a standard ER6. On a standard flycutter, you may need to grind a bit with a hook on the end to get the tip facing straight down.

[krems]

RRR,
Nice looking bullet moulds. I like your idea of making six block sets at a time. That must save a bunch of time. What kind of vise are you using that holds 6 block sets at a time??...It looks like a standard kurt vise.

What grade of aluminum / cast iron are you using for the mould blocks???

I noticed you are using a three pin alignment system. Are you stacking the block halves together when drilling the alignment holes? It looks like you are working on eack block half seperately. What material are you using for the pins??


Excellent job and post. I would like to make an adjustible bullet mould someday. I loved the pictures!...........Nice machines.

Krems

[Red River Rick]

Krems:

Making the mould blocks six at a time definitely speeds thing up. The mould halves are mirror imaged to one another, so basically you’re getting 3 matched sets out of setup.

After squaring up the material, it takes me four separate operations to complete each set of blocks. So once I’m setup, I usually make enough to make it worth while.

All the alignment pin holes are drilled and reamed at the same time. So once each mold block has been separated from its mate and the pins are installed, they are a perfect match. The handle slots are machined as well during this setup and the slots between each block (for separation) are done also. I machine to given depth which leaves approximately 0.100” of material at the bottom to hold everything together.

2nd & 3rd operations consist of drilling and tapping the holes for the sprue cutter plate, mould handle screws and adjustable base. And drilling and reaming for the sprue cutter stop pin.

4th operation would be surface grinding the exterior side of mould blocks. When I prepare my material, I leave about 0.005” - 0.010” on the thickness of my blocks. When I’m finished all my CNC machining, I place the unseparated blanks on the surface grinder and grind the blocks parallel to the spit line face. This ensures me that both halves of the mould will be exactly the same thickness. Sure helps when it come time to setup your blank blocks for machining the cavity after.

Last, would be to cut the mould blocks apart on the band saw, install the alignment pins, place each mating half together and machine off the tabs that held everything together.

My choice of material is Dura-Bar 65-45-12 ductile iron. It has some excellent properties that lend itself well for this purpose. No doubt, aluminum is nice, but certain grades just don’t hold up well to the repeated heating and cooling cycle. And beside, I have this material readily available.

Alignment pins are made from 3/16” hardened dowel pins. I machine one end of the pin into a ball-nose configuration or a taper.

Hope this info helps answer your questions.


Thanks.
RRR

[Greg5278]

Rick, the Durabar 65-45-12 is the same as I am using. It sure machines nicely,and gives a good finish. Did you check and see what type of grease grooves your tooling is capable of?
Thanks Greg

[montana_charlie]

I’m not sure how well people would take to curved vents though. They should work fine, but they may look funny to people that are used to seeing straight lines.
My NEI mould faces have curved vent lines.
They run vertically on the face, are very evenly spaced, and are about a 16th apart. They resemble the grooves on a vinyl LP record.

The way the curve lies on the face, it appears they were lying side by side (not end to end) when the grooves were cut. Reversing one block causes the grooves to 'cross' each other when hidden by closing the mould.

The arc of a groove is such that it is probably part of an eight to twelve-inch circle, and the arcs in the center of the face intersect the cavity all along it's length at intervals of (roughly) 3/32nds of an inch.

Anybody interested in using the Victory method of venting?
CM

[felix]

CM, what difference does it really make? Mirror image boolits being made is all I actually care about, well, except maybe for mold weight further down on the list. ... felix

[Greg5278]

I am using the venting method that Victory used to utilize. It is a precision ground trough /250-.500" wide, and .0005" deep across the bullet cavity. The .0005" depth ensures the bullet wil not "fin" when pored with high Tin bearing alloys. It will not pack up or attract dirt.

The NEI molds utilize a rough machimed finish, almost like a Fly cutter or a rapid feed with a big shell mill. It doesn't neccesarily mean quality, it just uses rough machining to make up for venting. In my experience, the small vent lines, like in Mountain Molds gets plugged, and must be cleaned.
Greg

[krems]

RRR,

There really is a lot of machining that goes into making the mould blocks. Thanks for the explanation.

Where do you guys buy the durabar 65-45-12 ductile iron?????..............The stuff sounds like it would make good mould blocks. I've always liked the Saeco mould blocks. I wonder what they use for their blocks. It looks like it has some copper in it.

Keep up the great work,

Krems

[truckjohn]

I am using the venting method that Victory used to utilize. It is a precision ground trough /250-.500" wide, and .0005" deep across the bullet cavity. The .0005" depth ensures the bullet wil not "fin" when pored with high Tin bearing alloys. It will not pack up or attract dirt.

The NEI molds utilize a rough machimed finish, almost like a Fly cutter or a rapid feed with a big shell mill. It doesn't neccesarily mean quality, it just uses rough machining to make up for venting. In my experience, the small vent lines, like in Mountain Molds gets plugged, and must be cleaned.
Greg

This is what I have been wondering about all along.

Production lead high volume casting dies don't use the little grooves anymore -- they use a completely vented parting line such as what Greg talks about.... typically, on big tools -- you go 0.0005" to 0.001" for the 1st 1/4 inch from the cavity, then it goes deeper -- 0.060" or so channels along the parting line and on out.

This helps stop weird voids and gas traps from forming all over the places..... and little bitty channels scribed into the steel are endless trouble -- as they stop up in about the 1st 5 minutes of casting.

These vents are precision ground, then draw polished to help them self clean. Cleaning is easy -- dry cotton rag or some scotch brite + a little degreaser does the trick.

Now, if I could only get a boolit casting mold cut like this too.....

Thanks

John

[Red River Rick]

Krems:

Your right about the amount of time needed to complete a set of blocks, from start to complete finish, probably close to a few hours. And the guys wonder why RCBS and others, charge $80 - $100 for a set of blank blocks.



I think the point here, regarding venting, should be, that it doesn’t matter what it looks like or how deep it should be, just as long as it provides positive venting without finning and nibs. I don’t care if you scribe pictures of naked ladies on the faces of your moulds, as long as it works, who cares.

Anyways, I’ve added a couple of more pics. Here is what 80 pair of mould blocks look like, their not all complete. I finish them off as I need them.

Regards,
Rick

[krems]

RRR,
Now thats a stack of bullet mould blocks..............Impressive to say the least. I bet you had a stack of chips built up when you completed all 80 mould blocks.

Nice photo's.............Does that Dura bar 65-45-12 change colors after casting w/ it over time or does it stay a silver color. Sure looks purty. The hard work is done....the easy part is cutting the cavity.

Krems

[garandsrus]

RRR,

Can I get a mold with a naked ladies venting patter? :) It would add a whole new dimension to casting!

John

[Greg5278]

Those Molds look just like mine, but a good bit more of them. I am also using an L shape alignment on the pins. They have 2 on the side by the handles, and one on the spue cutter side. The blocks measure 2.000" square.
Greg

[Red River Rick]

Krems:

If the blocks are left as is "in the white", eventually, they will change colour after some use. I bake my finished moulds in the furnace, at low temp, moulds come out with a nice dark brown patina finish, similiar to OEM moulds.

Garandus:

No problem. Send me a copy of the picture or that "certain part" that you want engraved on the mould faces.

RRR

[montana_charlie]

CM, what difference does it really make?
I don't know that it makes any difference at all. I was just describing NEI venting for JIMinPHX, to show that some casters are accustomed to seeing curved (rather than straight) vent lines...because he was wondering.

I am using the venting method that Victory used to utilize.
In my experience, that form of venting will almost blow your hat off when you pour the alloy in. I like it.
CM

[Red River Rick]

I like it.
CM

MC:

What do you like, the naked ladies or the venting?

RRR

[montana_charlie]

...getting my hat blown off...
CM

[Blammer]

naked ladies on the mould blocks?

gives new meaning to six banger or tapping the blocks, or....

so what GB bullet you gonna run on them blocks?

[Red River Rick]

I was thinking that perhaps I'd turn the whole lot into adjustable core moulds for swaging, shouldn't be to difficult.

Actually, I'll be using these for my PP moulds until I get my "cherri cutter" making skills down to pat. I'll have to stretch the next batch of blocks to accomodate 2 or more cavities, but again, that'll have to be later. As far as GB's go, that'll have to wait as well. But I do appreciatte the interest.

RRR

[HORNET]

RRR,
Looks like very nice work. On venting, you could consider full perimeter venbting like I've used on a couple of plastic injection molds. Use a small end mill to cut a trough about 1/16" out from the cavity with an escape path to the outside and relieve the surface between the cavity and the groove about .0005". Doesn't plug up easily but easy to clean.
What are those boolits at the bottom of post #29? Look painful to shoot...

[Blammer]

RRR, do you make any blocks that have boolits a dia of .625? Mabey with ONE lube groove? Truncone perhaps?

Or mabey .575 smooth sided Truncone or RNFP?

:)

[awguns]

Red River Rick,

Great thread.

Just curious as to why you have a $40,000+ Haas center in your garage? I don't mean to pry, but I would assume you have a business besides bullet moulds?

I am just jealous. I am not a journeyman (600 hours short), but I have been running CNC machines for the last 8 years (most of that time for the diecast die industry), and would be tickled just to have a manual bridgeport in my garage. Someday.

Smith

[Red River Rick]

Hornet:

I’ve seen that concept done on a few moulds, I think there is thread somewhere that shows a pic of that venting. Actually, when I cut that “Groove-Less” bullet, I did something very similar with the venting.

I too, have made many plastic injection moulds. I’ve never resorted to putting any venting on the moulds that I’ve machined. I’ve always relied upon what would pass by the ejector pins, never had any problems, yet.

Those boolits pictured in post #29 are 750 gr, 50 cal (0.510” dia) heavy weights. The intent here was to experiment with various lube groove configurations. Rather than machine a whole wack of moulds with different lube grooves, I made a mould that would cast a 0.510” bullet. I would machine various styles of lube grooves (width, depth, number of) into the blanks and then have a friend try them out. Saves a lot of R&D time, and requires fewer moulds.


Blammer:

Send me a PM, we can continue from there.


Thanks
RRR

[Red River Rick]

While waiting for the final coats of finish to dry on the mould handles for the GB, I found some extra time to spare and figured I better use it wisely.

I’ve been tempting my luck at cherri-making, and have had some really good results. Since I don’t have a CNC lathe, which would be the ideal machine for cutting the profile, I programmed my CNC Vertical Mill into thinking it was a CNC Lathe.

Using a carbide insert threading tool clamped in my vice, and the work piece (cherri-blank) held in the spindle. I was able to create a CNC program that performed the very same results as would a CNC lathe. The work piece moved rather the tool.

I’ve used D2 tool steel for making my blanks, my next step will be to cut the fluting x 3, heat treat and then hand grind the necessary clearances.

My intent here is not to make the cherri-cutters to a “As Machined Size”, but to a smaller diameter. For example: The first cutter (right side) is a .45/70 bullet design and measures at 0.400” in diameter. Using various programming methods, the final finished diameter of the cavity can be adjusted; you would not be limited to one certain size. If someone wanted that bullet design in 0.462” diameter and another mould of the same design in 0.459”, there would no problem. The same cutter would be used to machine both cavities, only difference would be final diameter.

So rather than having a large number of cherri-cutters to produce the same design but only larger cavities, one cutter will work, in this case.

This next project is of a 12 gauge HP slug mould, 760 gr. No cherri-cutting here. This attempt was done via 3-D surfacing. The only draw back is you cannot machine a “Sharp” inside corner due to the fact that a ball-nose end mill is used. So, the sharp edges of the front and rear driving band have a 0.032” radius instead of being sharp.

I ended up using a 1/16” solid carbide 4F BN end-mill for the finishing pass. Most of the material was roughed away with a 3/16” end-mill leaving about 0.010” for the finishing. For finishing, a smaller diameter end-mill would have reduced the inside fillet. On my next attempt, I’ll try using a 3/64” or a 1/32” BN end-mill. The draw-back with using a smaller cutter is “TIME”. The smaller the cutter, feed rates and step-over are greatly reduced, thus taking longer.

Just thought some of the members may be interested in this.


RRR

[IcerUSA]

3R's , them test blanks look good as does that HP mould . Have you gave any thought to a single flute cutter ? Thats what I'm working on for the lathe and was thinking that it would work well on a CNC mill with circle interpolation as you could helix it outward to your finished dia. and be taking a light cut so as not to have a lot of side flex .

Keith

[Buckshot]

...............Pretty fancy stuff there Rick :-) How come D2 Steel? That stuff is a cast iron puppy mother to machine.

.................Buckshot

[Red River Rick]

IcerUSA:

That single flute cutter idea would work fine if your hand grinding a cutter for one specific cavity and hope you never have to replicate that cutter again. I'm trying to come up with a method that will allow me to make cherri-cutters to a specific drawing or design. And then be able to reproduce that same design later on if need be. I think it would be next to impossible to hand grind one cutter and then try to duplicate that same design at a later date. With the CNC, once the programme has been made for a specific design, it can be easily saved and used again.

Buckshot:

Why D-2? I have a readily available supply of "off-cuts" that I collect from work, alot cheaper than having to buy it. The other advantage is D-2 Tool Steel is "Air Quench" steel, and makes things a bit easier when it comes time for heat-treating. No oil-quenching reguired, after removing the material from the furnace, simply let stand on a rack and cool in still air.

Your right about the 65-45-12 being easily machined. Then these D-2 cherri-cutters should be able to machine a lot of cavities before they start to show signs of wear or become dull.



I did manage to find a local company that has a CNC Tool & Cutter grinder. I've been in contact with them and I am currently waiting for some prices on a few custom ground cherri-cutters. They grind all their cutters on solid carbide blanks, price is not cheap but the quality and accuracy should be there.


RRR

[JIMinPHX]

...

My intent here is not to make the cherri-cutters to a “As Machined Size”, but to a smaller diameter. ...

So rather than having a large number of cherri-cutters to produce the same design but only larger cavities, one cutter will work, in this case.

... The only draw back is you cannot machine a “Sharp” inside corner due to the fact that a ball-nose end mill is used. So, the sharp edges of the front and rear driving band have a 0.032” radius instead of being sharp.



RRR

Interpolating with an undersized cherry should give you better cavity finishes too. Trying to take a cut with that much cutting surface is a bear, especially in something tough to cut like D-2. Even a good rigid machine like a Haas might cry about taking a cut like that. With the interpolation, you can adjust the chip load on the tool & smooth things out.

It’s been my experience that dead sharp internal corners in a mold sometimes make it tough to get good fill out when pouring a boolit. I think that your radius in there is an advantage & not something to apologize for.

Blocks that look like that & are made out of D-2 are better than anything that I have seen before, at any price.

My compliments to the chef.

[HORNET]

Dead-sharp corners at the bottom of the bands can also cause the bands to crack where they join the body diameter with the more brittle alloys. They also don't release the boolits very easily ay times. A couple of the minor disadvantages of the "pure" Keith design....

[Greg5278]

Hi Rick, I just got my 1043 Grain 12 ga mold back from a gunsmith. He bored the cavity to my specs, but the finish is a touch rough. I am going to send it out to get the air relief recut with a surface grinder. The mold is getting airbound, and the alloy does not want to flow in . I degreased it twice, and boiled the mold, and it helped. The other thing is running the alloy at 750F to increase the cooling time. That worked, but burns out the Tin.

The shrink factor for the Wheelweight and 2% Tin alloy I'm using equates to a .734" cavity, and a bullet dropping the Mold at .7295-.7297". That's the best I can measure with my mikes.

I'll send you a revised sketch of the mold, and a few proposed changes for another.
Thanks Greg

[Red River Rick]

Greg:

I was finally able to put the finishing touches on that mould. I haven't had the chance to cast any slugs, as of yet, but I'm hoping soon. One small problem, I now have to make handles to fit these "oversized" mould blocks, another project.

Those price quotes that I was waiting for (custom ground formed cutters) came thru yesterday, price per cutter is $245.00. I'm going to hold out for awhile and see what kind of performance will be achieved with this design before I drop a load of cash on the cutters. It would be a total waste of money if this designs proves otherwise.

I'll be looking for your new drawings.

RRR

[Greg5278]

Rick, I have not sent the drawings yet. I have to find the other sets of blocks. I only have one set left on my possesion.The others are in the Shop someplacein another state. I wanted to send 2 sets.

The HPpin looks good. I willprobably put it on a sliding bar, RCBS style, so it can pull the slug out of the cavities if it sticks.

I would hold off on the form cutters. Did you get any of the carbide bars I told you about? Perhaps Dave Manson at Manson reamerscould help you with the form tools.
Greg

[kodiak1]

Rick them thar moulds are just plain awsome. We will be doing buisness again a little later this spring for 2 more moulds a 40 and a 38.
You guys looking and kicking tires, Quit it and buy one you will be impressed.
Thanks Ken.

[andrew375]

When I made moulds I would use a fly cutter to true up and flatten the block faces. Then I would turn the rpms down, put on a 2 -3thou' cut and fast traverse across; super job!

Another idea I used was to wipe one block across some real course emery cloth. Just one pass, not enough to affect dimensions but just to leave a lot of deep scratches. It didn't look pretty but worked like a charm. This was on a mould I was given that didn't have any vent lines and refused all efforts to cast a decent bullet, five seconds work and she was dropping perfect bullets.

Excellent thread by the way.:drinks: