Tunnel gates in Aluminum molds

[mtechserv]

I build quick turn aluminum injection molds in my shop. Most of them are smaller simple molds for the cable / connector industry.

Typically, I use tab gates on my aluminum molds. However, I currently have an application that may require a tunnel gate. Does anyone have any input on machining a tunnel gate into an aluminum mold? On hard steel molds, you can typically EDM a tunnel gate. For my aluminum molds, I would like to find a cutter that would allow me too easily machine a tunnel gate into the cavity.

Any input on this issue would be greatly appreciated.

[Konrad]

I have made some very slender taper cutter for this purpose into 4140 H. material. For soft alum. molds you could make it out of drills.
Konrad

[caddyshack]

The problem with making these is that the tip usually has to be around .020. This is hard to hand make a cutter with a tip that small. We edm all our tunnel gates in house, even in aluminum.

[DavyD]

Depending on the size you could pilot drill a hole through and the use a milling cutter with 10deg per side taper to finish the gate. THe other option is to pilot drill then use a d bit cutter. If the gate is to be small you could use a truncated submarine gate or 'bucket' gate as we call it. You could take a standard slot drill (say dia1.5-2mm) in until half the diameter breaks through the cavity wall then finish with a tapered cutter. The truncated gate allows a greater volume of plastic to the gate area stopping it from freezing off too early.
Hope this helps.
Davy

[mtechserv]

Thanks for the input.

I've never used a tunnel gate in an aluminum mold before. I'm concerned that it will not hold up very long. I've used tunnel gates (.020" dia) in hard steel molds with no problems.
For my aluminum molds, I typically use 7075 or qc-7 alum. Typically, my aluminum molds are being used for flexible PVC. However, the mold requiring a tunnel gate will be used for Santoprene.

[Wiseco]

Check this usefull link

[MoldMaker]

We usually EDM all of our subgates, but in the "old" days we made single lip cutters on a Deckel SO type grinder or a harig.
http://www.gti-usa.com/pages/metal_deckel_so.aspx
You can purchase carbide split blanks for this. I have used pc's of broken endmills and such when really scrounging.
The great thing about the deckal type machine, is that you can grind a cutting edge on the bottom so there is no need for a pilot hole.
I have done .015 gates in Hi Hard P20 with these.

Ken

[rkonnen]

Sorry for such a late post. I cut sub-gates all the time in aluminum. I just use a 7deg. 1/16 or 3/32 inch end mill, usually on a 30 to 45deg. angle I only let half the tip dia. break threw,it leaves a "D" laying on its back shape.
REK

[TR MFG]

DME and PCS make sub gate inserts for use in molds

[mtechserv]

rkonnen,
I've heard of machining gates in the manner you have described.
When placing this type of gate in aluminum, wouldn't the lower edge of the gate (the bottom half of the endmill that didn't break through) break or roll outward?

[rkonnen]

I haven't see it. This picture even shows a little tit in the middle where the end mills center wasn't cutting. I am shooting 15% GFPP, works good. Now this is a steel core, I tried to take pictures on an aluminum one, to shinny, couldn't get a clear picture. I am not saying subgates that have all the proper angles in them do not have a place, but from what I have seen of other mold makers work , I have not seen any that have done it the text book way. All have their own little spin. Also with the aluminum, the sub gates running GF does tend to wear on them, so I mainly use for low volume or put a steel insert in for the gate.

[Jim Estes]

When I was just getting started in moldmaking, one of the jobs that I was tasked to do was to cut gates into S-7 steel hardened to 52-54 rockwell C. We made the single lip sutters with the Deckel grinder and then we would set up in a Bridgeport mill, kicking the core block up to 45 degrees, and then locating the gate location and lock the table down. Then crank the speed up to 2500 rpm and take a 0.001-0.002" cut per peck of the quill. After about 2 holes anyone can do it. The bad part about this is that when you break the tip of a cutter off in the bottom of a gate, you have a hard time getting it out, but this is still quicker than EDM, and it doesn't tie up an EDM, just a mill and a warm body. We would typically do this for the 16, 32, 64, and 128 cavity molds. Either way there are problems, usually when trying to EDM a tunnel gate, or subgate as we called them, you couldn't get the flush to work just right to flush the tip of the electrode so it slowed the burn.
These days I usually try to mill my gates first and only burn them if I have to.

Jim