Moldmaking basics?

I've agreed to run a set of injection molding plates on our CNC mill. This is for a prototype mold for an ABS case, two sets of two plates made from aluminum. The customer, another university department, is writing the code and even supplying the tooling, so I don't have too much to worry about.

Except that the collective moldmaking experience between all of us is about 40 hours that I had way back in a previous job. I'm fine with draft angles, pins, and so on, but they're asking if I agree with their tooling choices and toolpaths, and I can't give them much help. They realize that the risk is all theirs, but I want this to be successful and feel I need a bit more base knowledge.

Some specific questions:
- What's the best way to create corner fillets at the bottom of the mold? I'm thinking multiple passes with a ball end mill smaller than the fillet. They want to go one pass at the ball radius.
- How about blending the fillets into a flat floor? Use the same ball end mill to cut the floor, or a square end mill?
- How large of tool marks can I reasonably leave for hand work?

Please don't tell me I should farm it out--it's not that kind of job. But if there are other pitfalls I should know about, I'd welcome the input.

I would use a ball end mill smaller than the radius if you can, that way it will always be cutting, and will probably give you a better finish. You could cut the floor with either a ball or a flat cutter. Ball if you want to do it all in one program with no stopping. Flat would probably give a better finish on the floor, and faster than using the ball cutter on the floor. Who has to do the polishing? If it's you, I would let the program run at night with a very small stepover, this would lead to very little handwork for you to do. If it's them, and you want to get it out of your machine as soon as possible, give it more of a stepover (keep the scallops at .001 or less), and they can easily finish that in aluminum by hand. Use paper on a polishing stick, not stones for polishing the aluminum. Polishing stones will plug up with aluminum.

Remember to add shrink, draft, and venting as necessary. Water lines?

Another option for a cutter would be a bull nose end mill. Depending on the corner radius, with the right amount of step over you will get a nice finish on the sides as well as a smooth finish on the bottom of the cavity. Wet and dry sand paper works well for polishing with a squirt of WD 49. Good luck with your project.
Rolf B.

Thanks for the tips. The bull nose sounds like a good idea. Would it be better to finish the walls with a tapered end mill, or the same bull nose with a small step-down?

There is a simple coolant channel that will be drilled in from the sides. Inlet, outlet, and cross passage that will be NPT tapped and plugged. I don't see any problems there.

Tapered endmills can be used is you have the right angles and can properly program for them. Since they are generating the code you are kind of at their mercy for what tools they buy.

You do not say what type of aluminum you are using for the mold. If at all possible I would try to use 7075 or 2024. 6061 works but you have that chance of getting some real gummy stuff.

I agree with the other guys about using a smaller radius ball mill or bullnose mill for the fillets. Mulitple passes. Mulitple passes. Mulitple passes.

I don't know whether the part is very '3D' or 2.5D in form. This has a lot of influence on how easy it is to finish. Flowing lines and curves will take a lot more passes to finish. For larger areas of curves and flowing line I would use as big of a radius ballmill to minumize your cusp height as this will have an inlfuence on the amount of finishing required. Plastic does show all the scratches and marks so depends upon what the final part appearance need to be for overall finishing.

If you are going to use an inserted mill make sure you only use ground/polished inserts designed for aluminum.

Do not leave square corners or bottoms. Meaning all joints should be rounded or filleted. Sharp corners induce stress into the plastic and can cause the part to fail. Everything needs to flow without turbulence.

It used to be that the CNC jockies would cut the sides and the bottom of the cavities and then we'd set up on a BP with a Quillmaster and pick out the corners. The Quillmaster lets that ball-nose mill run at an angle instead of vertical and gave a much better finish.

One thing that I learned while making molds; The guy that machines the cavity never gets a good enough finish for the guy that has to polish!
JR

DME has free online moldmaking info.
D-M-E Plastics University® - Online Courses

They have alot of good basic information.

If you're going to be polishing the mold and not very experienced at it...you may want to leave .010" on the parting line surface to finish machine after polishing.
This will give a nice crisp cavity edge.

If the toolpath is written to start on the parting surface and roll down into the cavity and back out, you may also lose some of the cavity edge.
Depending on the software and machine accuracy/speed.

I usually programmed the cavity path separate from the parting line path.

Depending on what kind of rad your looking for and the cavity depth you can sometimes use a split cutter with the correct draft you're looking for with the radius on the tool as well for a finish pass , i realize that depending on the design it may not be the correct way to do it , but just a thought.

Thanks for the help. We did a trial run in some leftover 6061 that went fairly well. (The real plates are 7075.) There were a few spots where tools didn't blend into each other very well--the fillets to the flat bottom have about a .002 step. But overall, pretty good.

I like the idea of leaving .010 on the parting face to finish after polishing. It also sounds like a tapered bull nose end mill would be a great tool for cutting walls, fillets and bottom without having to change tools. I can find them as a custom, but haven't yet found anyone stocking them.

The tapered endmill is tempting for cutting a core and cavity, but keep in mind that will leave you a conical radius in the corners, MOST of the time in moldmaking, at least from our customers, there is a constant radius in the corners with draft, so what that means is that you would have to go back into the corners of the cavity and remove some material with a bullnose tool and step them out to make them the correct size. On the core side, you would be missing stock. Without seeing your part it's hard to say, just something to keep in mind.. Oh and one more thing, the plus stock on the parting line that was mentioned ealier is a very smart idea, we do it on all our molds, even with a good polisher, they think they can keep a sharp edge, but in reality most people just cannot.