[DomB]

Hi there,

I was just wondering how I would go about accurately setting the length of the ejector pins in a plastic injection mould.

My first instincts are to put all the pins in the mould with the plate retracted and mill the cavity in one and the pins will be machined with it. However will the ends burr over making them stick. I am making the mould out of aluminium so a hard steel ejector pin in the middle of a lump of ally would be like your rip saw finding a nail in a chunk of wood! And would you set aluminium feeds and speeds or steel feeds and speeds?

Do I add the pins to the core after? If so would it be recommended to drill from the back of the mould plate breaking into the mould area, or drill in from the mould core/cavity area through the plate risking damage to the cavity?

Or perhaps drill the ejector pin holes first before anything is cut? Or would all these holes cause many interupted cuts playing havoc snapping my tiny mould finishing cutters (0.2-0.5mm).

If I drill them after the cavity is cut, how to I make them an accurate length so as to leave as little marks on the part as possible? What sort of length accuracy am I shooting for 10-50 micron?

What if the end of the pin is not flat but forms part of the mould contour? Does this ever happen and therefore require pins that do not rotate in the holes?


Can anyone shead any light on this mysterious side of mould making.

Using a Haas VMC/solidworks to make the mould. Have made simple moulds before but none with an ejector mechanism other that my fingers!

And yes I am spelling Mould with a 'U' as I am british.


Dom:drowning:

[Leehound]

I have done hundreds maybe thousands of ejector pins. So I will try and shed a little light on how I do it.

I build Investment Casting molds (no U in my molds), so the mold base is aluminum. I always drill and ream for ejector pins "after" all the cavity work is done.

9 times out of 10 I will drill from the back side of the mold base. I clamp the ejector plate to the back side of the base and drill, ream and counterbore all in one setup. If you have a base that is very thick or you are drilling for small ejector pins, a wandering drill might be a concern. Then you might want to drill and ream from the cavity side and then I might open up the hole a bit from the back side.

After all my holes are done, I will assemble the mold. With the ejector plate in place, I will depth mic through the ejector holes and establish all ejector pin lengths.

With my pins and dimensions in hand I head over to the surface grinder. I have an ejector pin fixture for the next steps. First rough length is established with a cutoff disk. Then I grind the tops of the pins to the correct lengths.

Sometimes pins are located in a non-flat or contoured area of the cavity. In this situation I will "time" the pin by cutting a "D" shape on the head. These pins must not rotate. In the ejector plate, instead of a counterbore I will machine a matching "D" shape. I assemble the base with pins in place and machine the top of the pin to match the contour of the cavity.

I try to establish the lengths of the pins with "metal safe" in mind. If I make a mistake, I want them to be too long and "not" too short. Although I try to establish the lengths dead on, my customers would rather have the pin impressions on the "part" to be slightly recessed rather than raised. The tolerance that I try to follow for the length of the pin is: - .000 + .001 (inches of course)

Hope this helps.


Scott

[DomB]

Thanks Scott,

thats a great start very helpful information. It's surprising how little information there is about this sort of thing outside of mould shops on the internet etc. It's only when you try to make a mould that you start coming up against these hurdles.

Another couple of questions, do you use split ejector plates to hold the head of the pin?

When you machine a 'timed' contoured pin, do you have to pour wax or simmilar in the pin bore to hold the pin to stop any play due to the space allowed for venting down the pin bore, to stop the pin rattling whilst you machine it?

Or do you machine the pin contour out of the cavity using the cad/cam system toextract just the little piece of contour onto the end of the pin?

With regards to venting, do you leave a clearance around the whole pin or do you grind a flat along it?

To mike up the holes do you have any sort of special tool to deal with the very small pin diameters?

Many thanks
for the helpful relpy

DomB

[Leehound]

Thanks Scott,

thats a great start very helpful information. It's surprising how little information there is about this sort of thing outside of mould shops on the internet etc. It's only when you try to make a mould that you start coming up against these hurdles.

Another couple of questions, do you use split ejector plates to hold the head of the pin?

Yes, I use split ejector plates. The top ejector plate is drilled, reamed and counterbored. The bottom plate is what the pins sit on.

When you machine a 'timed' contoured pin, do you have to pour wax or simmilar in the pin bore to hold the pin to stop any play due to the space allowed for venting down the pin bore, to stop the pin rattling whilst you machine it?

I always ream .001 over the size of the pin. And carefully counterbore .001 deeper than the head of the pin. It's important not to counterbore too deep. With both ejector plates bolted, the counterbore should allow the pin to rotate freely, but not allow any up and down movement. With those tolerances the pin is snug enough to machine, but I am careful and take small cuts.

Or do you machine the pin contour out of the cavity using the cad/cam system toextract just the little piece of contour onto the end of the pin?

I use Mastercam for programming, and isolate the cutting only to the end of the pin.

With regards to venting, do you leave a clearance around the whole pin or do you grind a flat along it?

I "do not" vent ejector pins. With Investment Casting molds, all the venting is done at the parting line.

To mike up the holes do you have any sort of special tool to deal with the very small pin diameters?

If a hole is too small to depth mic, I will just depth mic from a larger hole location to the smaller hole and do some math.

Scott

[spider]

this is what i used to do when i was on the floor;

with the core cut, i'd messure the perallels (rails) and stop buttons, and figure out my packing (between the ejector plates and core). I'd then put the ejector plates on the back of core with packing (123 blocks and shims +.050 to be safe). after securing the plate on with couple of clamps and return pins i'd flip it on it's side and add the rest of the pins. Go to the front of the mold and push the pin back till they are flush with the molding face, then go to the back and scale how much the pin is sticking out past the plate......chop it off on a saw.... Later on i'd assamble the core, put the Jackscrews in (and pull back screws) to make sure the plates are back, and then i'd grind the pins flush with a disk.....or give it to my polishing guy to blend the pins....lot of times he has to get a head start on polishing anyways.......on a medium size mold it can be all done in a day.

as for venting, i make a setup on a surface grinder and grind .001 for about 3" down, on 3 places around the pin. once you set the height, no need to change it, just place the pin and move the table once and it's done.....

all our pins are D-locked. we usually rough out the flat on a bench grinder and then make a setup on a surace grinder to finish it......make one stup....eyeball the flat horizontal.....bring in the wheel and grind it (almost tangent to pin dia.).....DONE!!!!
plates holes and pockets are done CNC, with .031 clearence in the holes in plates (makes the ejection go easyer....ejector guides keep it going straight....if the pins are reamed in plates SOMETIMES they fight eachother)

as for miking the holes....never done it....
I send my ejection to be "gundrilled" and it's usually close enough....sometimes i trow a reamer in the hole by hand just take the burs off if there are any....Cheeper then doing it in house.

[DomB]

Thanks guys, again really useful info. Looks like this is a whole new art to learn.

Dom

[lerman]

I just spoke to my father about this problem (he's a moldmaker with 50+ years of experience).

Some suggestions:

1 -- If you need to keep an ejector pin from turning, (as others have said) grind the head to a Dee shape. What he used to do (this was before CNC machining), is mill a slot in the holder and insert some keystock to keep the head from turning.

2 -- My father did zinc and aluminum die casting. Ejector pin maintenance was a big expense. Metal would get into the space around the pin and hang up. To avoid that, he would hone the hole rather than simply reaming it. The smoother finish would keep the metal from getting caught on it.

Ken

[DavyD]

Hi Dom
I am a mould designer/maker based in Scotland so also spell mould with a 'u' !

We usually drill and ream our ejector pins holes from the front before any core or cavity detail has been cut. This means on a flat plate you can centre drill all your holes first as they are all on the same plane. This is probably the most accurate way of positioning them relative to the mould cavity.

Most of the pins we use are below 12mm dia. and we drill first with a drill 0.2mm below the reaming size. We then ream to the nominal size of the pin. Ejector pins from DMS and Hasco are usually 0.025mm below the nominal size so reaming should give a good sliding fit and the clearance is usually sufficient for venting.

The length of ream fit is typically 5 x pin dia. for up to 4 or 5mm and maybe 2-3 times for larger dia. Too long a reamed fit will prevent venting.

We then turn the plate over and drill a clearance hole (0,5mm dia. greater) up to meet the reamed hole from the front. We also countersink the clearance hole at the back to provide a 'lead in' for the pin.

Doing all the operations from the back means less set up but we usually find that we cannot get long enough reamers to go through the plates. Also drill wandering can be a problem for accurate position relative to the cavity/core.

Machine reaming in aluminium can be tricky and we find sometimes holes cut oversize - if you only have a few holes hand reaming may be more accurate.
To size the small ejector pin holes we use pin gauges.


I've just noticed that you are using very small milling cutters and ejector pin holes may cause problems with cutters wandering into holes and breaking. It may be safer for you to drill and then hand ream from the back of the plate.

We use split 2 plate ejector plates as supplied in standard mould kits. We drill a clearance hole 0.5mm larger than the pin and a cbore for the head 0.5mm larger. The depth of the cbore should be 0.05mm deeper than the head thickness. The pin should be able to rotate when the plates are assembled. We sometimes ream the push back pins in the ejector plate but for alumunium moulds we often use ejector guides to prevent 'firing up' of the ejecting assembly.

If you have a pin which needs keying there are a number of options. Grind a flat on the head and locate it a matched D pocket in the plate or mill a slot and lay in a keysteel pin to locate against the flat ground on the head. Alternatively, drill a small hole in the side of the head and fit a timing keysteel pin which locates in a slot.

With regards cutting the form on the pin you can buy soft pins which can be milled but we usually spark erode the form or grind it by hand using a die grinder.

To cut the pins to length we assemble the mould and determine the overall length from the back of the front ejector plate to the split line. We then determine the length of each pin and first rough cut them to length (0.5mm long) using a 'cut off' wheel on the surface grinder. We then finish grind them to length. Be careful not to grind too much off as the small surface area of the pin can heat up and the pin length expand. Let the pin cool down between cuts - use a piece of copper to sink the heat out of the pin between cuts.

To hold the pins on the grinder you can clamp a 'v block' to an angle plate and lock the pin in position for grinding the front face. Place a slip block on the mag table and sit the pin head down onto this surface as a stop. You can then alter the size of the slip block to suit the different pin lengths required.

Hope this helps

Davy

[DomB]

Thanks Davy, and a happy new year to everybody (soon anyway).

The information is truly useful, I am getting closer to understanding this art step by step.

I think I will be using DMS pins as they are just down the road from me in High Wycombe. I will try and get plenty of questions in when I visit them.


Is it not normal to use very small milling cutters like 0.2-1mm?? Without a sparker it seems the only way to get the detail and finish, on the small rads of the cavity.


Thanks again
Dom

[DavyD]

Hi Dom
We try to avoid sparking whenever possible and if we can finish mill a core/cavity we do. We try to advise our customers on part design that suits milling i.e filleted corners etc. This means we can make their tooling cheaper. Quite often part designs have features that require sparking but are unecessary to the function - so we suggest a milled alternative. CAD designers can get carried away with the functionality of their software and create unecessary features that add loads to the tooling cost.

However sometimes you can't avoid using very small cutters. We have bought a high speed spindle for our mills which gives us 40,000rpm - this helps. The other problem we have is getting small cutters that have long enough reach to finish the bottom of cavities. They are available but are expensive and easily broken.

It cetainly worth discussing the part designs with your customer and trying to come up something that satisfies their needs and is easy to mill. They usually like saving money !.

Regards
Davy