Building a Die Casting Mold (Soap Dish Mold Part 1)

This is my granddaddy project, the whole reason I chose to go to school for tooling was to be able to make permanent casting molds for my foundry.  Unfortunately, the information I learned from the tooling class helped little with the mold making process.  Even the internet has low to no information on mold making, well at least not in English, so I had to learn from word of mouth.... It isn't that complicated actually.  The only difference between this and a sand mold is instead of sand it will be made of steel.  How hard can it be?

As mentioned in my evil plan, the mold is for a soap dish.  I started by taking the dimensions of the soap dish and finding a piece of steel that will give me adequate room to make the cavity.  The problem is, the only thing I could find was a round piece 6" in diameter 8" long.  This meant I would have to machine it square-like and cut it in half for the 2 halves of the mold.

The first step was to put it in the lathe and face the ends clean so it would fit in the mill vise correctly.  I had to use the biggest lathe in the shop to fit this monstrosity.

My tool bit looks so small compared to the piece!

After a few hours, I had cleaned up the faces and periphery, though I could've gotten away with just facing it.

Next, I put it in the milling machine and fly cut the top flat.  I did this to make sure the saw blade wouldn't wander around when trying to start the cut, also for a locating surface.

I milled flats on the sides in the same setup using a long endmill, this way I have 3 surfaces that are perpendicular to each other.  I then flipped it over and faced the other side.

Coincidentally, the day I needed to cut this thing, the school got a brand new horizontal bandsaw!  I knew with this kind of luck the mold was destined to be a success.... we'll see.

The cut was really straight, not bad for the first time using it.

Here are the halves after the cut.  One side is bigger because it is going to be the protruding half while the other is the cavity.

After much more milling, the parts are ready for the CNC.  It's about time, there's only a little over a week left of the semester and I barely have my stock prepared!!  I've been working night and day (well, just night) to get my CNC program done to finish this thing.

UPDATE 5-22-13

Well, finals week is half over and I finished the first half of the mold.  So far so good, here's a recap of what happened:  (non machinists can skip this section and scroll down to the pictures)

• Day 1:  set up the CNC machine,  assembled all the tools, offsets etc.  First I faced it and drilled the holes.  Started roughing out the pocket with 3/4" high speed steel endmill.  Wrecked the cutter half way through the operation, either due to too high spindle RPM, or because I put it in the collet incorrectly or both.  I had turned up the RPM from about 500 to 1200 though the proper cutting speed was 500.  I did this because when I saw the face mill RPM was 170 I thought it was a joke because we run them at work at 1000.  Therefore, I started to distrust the speeds and feeds Mastercam put in my program even though they were "proper". 
  After that, I was given an indexable carbide endmill to use to finish the rest of the pocket.  This worked out well except that the tool wasn't suitable for the finish pass because it required a tool flute length longer than the carbide insert.  I then switched to another HSS endmill, this time I ramped the RPM up to 1800.  It was cutting funny because of the speed, so I fed it in slow.  It then ramped down to finish the bottom of the pocket and it started getting loud.  I stopped it and checked what was happening.  It was at this point where I restarted it that things got questionable.  I have 3 people that can testify that I accidentally turned on the spindle backwards, but how am I supposed to know whether or not I accidentally pressed the wrong button, if I was aware of it, I would've not done it.  Anyways, the machine started sounding and shaking like an earthquake.  I let it run for a while, stopped it, and took out the tool to look at it.  The end of the tool looked like it had been melted and smeared all over.  It left a very crazy, crackley surface finish on the piece as shown below.

crispy and crackley

I then talked to the old guy in class about what happened and how I was running 1800 RPM, his response was hilariously vulgar.

• Day 2:  I got a hold of that indexable endmill again so I could finish the rest of the pocket.  After what had happened, I decided to look at the speed/ feed chart because I wanted to do this the right way.  It confirmed that the speeds and feeds that were in the program were indeed correct and that I was an impatient bastard.  After that, it changed to a 1/4" endmill to do a "rest mill" operation, in which it cleaned up the pocket corners and roughed in the draft angle.  After that, it switched to my prized 3/16" soiled solid carbide ball endmill to mill the bottom fillet which I had to do twice because the tool height offset was incorrect.

Machining the fillet radius, I used the "bathtub of coolant" method.

• Day3:  Put in the 2° tapered 1/4" endmill to mill the side of the mold so when I pour in metal I'll be able to get it out.  I accidentally ran it into the corner too fast and it left a few gouges in the side.  Oh well, that'll be a few more seconds of filing each part after being cast.  It's not bad enough to be a FUBAR yet.  I could've stopped it there, but I wanted to have my company name embossed on the bottom of each casting.  That posed a problem since I don't have a company, so I just used the name of this blog, Green Furnace Foundry.  I also milled a loop around the bottom for the soap dish to sit on as opposed to the letters.  I used the 3/16" ball mill to do the engraving.  I didn't engrave "Made in U.S.A." on there because that is played out.  I did consider putting "Made in USSR" as a joke, but I ain't meeting any quotas.
  I got the idea one day when I was looking at the bottom of plastic army men, I saw the word CHINA and the "N" was backwards.  It occurred to me that they were too cheap to get a backwards letter "N" stamp.  I looked up how much backwards letter stamps cost, and just like everything else backwards (like left-handed taps and dies), they were 3 times as expensive as the forwards variety.  I decided it would be easier to just engrave it, so I engraved it backwards.
  

Engraving

All done for now, I will still have to cut the runners in and ejector screw holes and probably ejector pins too.

I'm really looking forward to milling the next half. It looks like it's going to take a fortnight to machine though...

UPDATE 5-25-13

Today was the last day of class, and.... the mold isn't finished.  So much for that pizza party I was going to throw.  I did, however, get the second half 7/8 complete.  Here's the summary of what happened:

Set up the machine with tools and offsets etc.  Forgot the flash drive with the CNC program at home.  Got back, loaded it up and started roughing the shape with 3/4 indexable endmill.  When I say roughing, I mean taking the piece from this:

 To this:

 And so on...

Eventually getting the core shape complete.  I started out at 1200 RPM to do it the "right" way, my teacher walks up and asks why my RPM is so low.  Well, I ended up speeding it up to 3000, and for good reason.  I hadn't realized the cutting inserts were not suited for cutting steel because of the excessive positive rake angle, so cutting slower wore out the edges faster.  Positive rake means the sharp edge is pointing towards the material being cut, I think of it like an ice cream scoop.  When the rake angle is too high when cutting harder stuff, the edge breaks down faster because it isn't as strong.  A negative rake angle cutter probably wouldn't have been preferred in this operation either because they are for really hard or tough material.  Refer to the poorly drawn diagram.

Anyhow, I didn't realize this until after I had wore out the first half of the inserts, so I flipped them around, sped it up to 3000 and the results were satisfactory.  The higher RPM meant less material was being cut per revolution, therefore minimizing tool wear.  After about 3 hours, the core shape was done, and then the dowel holes were drilled and reamed.  I have a funny feeling they aren't even going to line up with the other half...

Center drilling

Reaming to 1/2" after drilling 31/64"

 Next, it roughed the area where the knobbly bits go, first with the 3/4" endmill and then a 3/16".

After the 3/16" cutter was done cutting, it kept doing some unnecessary movement and was wasting time, so I decided to stop the program and resume it on the next operation. BIG MISTAKE, I forgot how long the CNC program was and I ended up having to scroll down 20,000 or so lines in the interface to find the next start point.  I thought after that they would need a new "page down" button for that machine.  That's the disadvantage of using advanced CAD/CAM software to make the CNC program; it generated a MASSIVE 1.3 mb text file, which is a lot of text.  The code was so huge I couldn't even copy it onto the machine's memory, which led to the downfall of the final operation.
The second to last operation was milling the tapered wall and a shallow pocket so my parting line isn't on the top edge of the soap dish.  I did that because I had intended to mill a .030" radius for the top edge, but my tool didn't get a nose radius so I just left it sharp.

Milling the tapered wall.

Next was the fun part, milling the 3D contours of the knobbly bits and the top (bottom) radius .003" at a time with my 3/16" carbide ball endmill.  I took the advise of the guy at 23b and sped the RPM up to 8000, and it cut excellently.  Since Mastercam made the code so unnecessarily long, for one arc move there were about 20 lines of code.  This made the machine get a bit jerky when it went around the corners because I had increased the feed rate, and the machine had to comprehend that much code that fast.

The maximum spindle speed is 8100

Though my time was running out, the operation was going smoothly, and it appeared it would be finished today.  Unfortunately, in the middle of the operation, there was a memory fault, as if the flash drive had been disconnected.  Well, the flash drive was still there, it must've got tired of reading the code.  This wouldn't have happened if I were able to copy the program onto the machine's memory. There clearly wasn't enough time left to find where it left off, let alone if I could even get it to load the program again, so the mold remains incomplete.

Oh well, I'll just finish it during summer session.  Check back in a month or so.

Update 7-1-13

The second half of the mold is now finished!  All I had to do was open the CNC program in note pad and delete the first half that has already been completed, and re save it as a different file.  It did, however, need to start at the beginning of the last operation.  This meant I'd have to sit through it going around and around cutting air until it got to the point where it had the error.  Not a big deal, I just put the feed override to 999% to make it go faster until I heard cutting and slowed it down to a reasonable rate.

After the knobbly bits were done, it went to do the outer radius on the edge.

Then, a final operation to clean up the leftover metal in between the knobbly bits.

Notice how yellow the coolant is now

And then, after countersinking the holes, it was done!

I need to get some real glamor shots of these taken

I started polishing it with an India stone to remove the flat parts at the top of the knobbly bits as well as removing the tool marks.  Don't want the soap dish to get stuck in the mold.  Also to remove any imperfections like the corners that seemed a little too pointy.

I tried to choreograph the entire machining process to make the mold halves appear equally sized when put together.  I think it's convincing enough.  You won't believe the amount of math it took. 

So until I can cut the runners and find a place to use the foundry, this is where the mold will be.  Though it appears I will need a stronger shelf to support the weight.

Part 2