Advice For First Mold Job - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 40 of 40
  1. #21
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,830
    Post Thanks / Like
    Likes (Given)
    1092
    Likes (Received)
    1134

    Default

    Quote Originally Posted by TheWolfOfWalmart View Post
    Luckily none of that is really anything I have to worry about on this job but I appreciate the context as to some of the things that has to be considered at a higher level
    OH, you might be surprised to find out they do matter.

    Simple part in P20 doesn't make sense to me, unless millions of shots are expected.

  2. #22
    Join Date
    Apr 2006
    Location
    Suffolk, England
    Posts
    876
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    233

    Default

    Quote Originally Posted by TheWolfOfWalmart View Post
    Can you clarify what you mean by this? And yeah I really think this is a simpler part than it seems people are thinking, which is on me. Probably because small-fish me hears 'mold' and sees things much differently than all you guys that have been doing this since before I was born lol.



    No talk of pins yet so I'm not really sure if/when/how that will come into play as far as this job is concerned.
    Inserting simply means cutting the cores and cavities into a separate block of steel, which you then insert into a pocket in the bolster plate. So if you have to remake it, you just need another smaller block rather than a whole mould plate.

    By pins he means ejector pins. You will need them, unless it's a 3-plate stripper mould

  3. #23
    Join Date
    Mar 2011
    Location
    Geneva Illinois USA
    Posts
    6,134
    Post Thanks / Like
    Likes (Given)
    2590
    Likes (Received)
    2379

    Default

    Terms A mold is the complete unit, with cavities, cooling/heating, ejectors..everything. A big block of steel that fastens to the molding press. A cavity is just the part of a mold that makes the part, usually inserted into a mold base. The mold base has everything except the cavities. For small simple parts the mold may be the cavities with suitable clamping and gating. They often don't have ejectors, heaters or such and are intended to proof of concept.

    Tom

  4. #24
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    2

    Default

    Quote Originally Posted by Peter Neill View Post
    Inserting simply means cutting the cores and cavities into a separate block of steel, which you then insert into a pocket in the bolster plate. So if you have to remake it, you just need another smaller block rather than a whole mould plate.

    By pins he means ejector pins. You will need them, unless it's a 3-plate stripper mould
    Quote Originally Posted by TDegenhart View Post
    Terms A mold is the complete unit, with cavities, cooling/heating, ejectors..everything. A big block of steel that fastens to the molding press. A cavity is just the part of a mold that makes the part, usually inserted into a mold base. The mold base has everything except the cavities. For small simple parts the mold may be the cavities with suitable clamping and gating. They often don't have ejectors, heaters or such and are intended to proof of concept.

    Tom
    Ohhh. That would make sense here. I've seen a full stack of mold plates for his machine in particular and they are much bigger than the piece he is having me machine the cavities in. The halves don't have any holes that a pin could eject the part through. Just the cavity, a flow gate, watercooling channels, and orifices to the cavity for the core and cavity core pins. Still waiting to hear back from him.

  5. #25
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    175
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    96

    Default

    FWIW, I've designed 6 injection molded parts. The steel one was for a thin folding case with a living hinge at a cost of ~30k. The material had to be polywarpolene due to contact with chemistry. Took a couple tweaks to get it perfect, and these were guys that do it every day for a living.

    The other 5 were done using soft tool aluminum molds (protomold) at around 6k, and good for a couple thousand parts. They include 20 or so parts with the initial cost, then a few bucks each for however many you want.
    The parts were abs with about .09 thick walls (2 shells that screw together). Part assembled was 7 x 4 x 1.8.

    If your not making a ton of parts, I would go with soft mold (also referred to as bridge tooling)

  6. #26
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,543
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1980

    Default

    Hi again TheWolfOfWalmart:
    I believe I'm getting closer to an understanding of what you're being contracted to build here and if my guesses are correct, the things you will need to consider are somewhat different to what we've talked about so far.

    So: could your customer perhaps be running a Morgan press or some other similar prototyping press?
    If so, the requirements for a mold are quite different from what moldmakers are accustomed to, principally as regards the mold design.

    For those of you unfamiliar with this kind of press, it's an upright (a bit like an overmolding press or an old style Arburg All Rounder) with platens arranged in the horizontal plane and the Hotside on the top.

    These are dirt simple machines good for the garage or the prototyping lab, and are not really intended for any kind of volume production.
    They are not equipped with a knockout system so if auto ejection is desired the ejector plate is usually pulled with bars or chains from the hot side.
    Molds are often not even clamped in the machine but are simply laid on the lower platen that has a locating feature and a simple toggle to clamp.
    The lower platen moves upward.
    It's a 20 ton machine so it's pretty small.


    Mold design is quite different for these machines from what a "real" mold looks like and how it works, so if I'm right about this guess, much of our babble about the principles and practices of mold design is irrelevant for this particular instance.

    So let's get to the heart of what the OP is asking about:
    You want to know about what to be aware of milling mold cavities in P20 with a Haas Minimill.
    Somewhere in the conversation, Fusion 360 was mentioned and it sounds as though the customer may have provided the programs and all you're supposed to do is cut the shapes based on his CAD work and his CAM work.
    Is that all correct?

    So my questions follow:
    First, do you have your own seat of Fusion?
    Second do you know how to run it for 3D milling?
    Third, have you ever milled P-20 before?

    The availability to edit on the CAM side and to re-write the code to suit your own practices will be crucial to your success especially if you have to run small cutters with long stickouts.
    P-20 is pretty tough; think 4140 HTSR but a bit harder, maybe low 30's Rockwell C.

    A Minimill is a capable machine for this kind of work but suffers from two significant limitations (I have one and I use it for moldmaking so I can speak to this subject with fair authority)

    1) the maximum spindle speed is 6000 RPM so if you are running cutters less than 1/6" diameter, you will need to run pretty slowly to avoid big chiploads, and finishing even a tiny cavity to a decent standard can take HOURS.
    This will heat up the machine pretty good which brings me to point two:
    2) The machine is not thermally stable and is much worse in Z than in any other axis (although it's not great in Y either)
    So you must either accept the errors or work around them and that is possible but time consuming and not easy.
    If I run my Minimill from warmed up for 3 hours at 6000 RPM I'll have grown 0.001 in Y and 0.0015 in Z but X will be within tenths.
    All C frame machines do this to some extent, but a Minimill does it badly enough that it is an issue if you need things to line up decently when the mold halves come out of the machine.

    On a core-cavity mold it often doesn't matter a damn, but on a cavity-cavity mold it's enough that the parting line on the part looks like shyte unless you compensate for it.

    Often times you can get around the errors to a significant extent by mounting both mold halves side by side onto the mill table at the same time set up like pages of a book, so that as the Y axis drifts both halves are malpositioned in the mold by the same amount.
    If you rough both and then finish both cavities with a warm machine you can do quite well.
    Whatever you do , don't finish one cavity in the afternoon, shut down overnight and then finish the second cavity next morning...you MUST run both to completion before you shut down for the day.
    Ditto if you need features within the cavity to be accurately positioned with respect to each other.
    Don't run one feature yesterday and another today if you want them accurate...on a Minimill it just won't happen!

    Next topic, toolpaths and cutters:
    I run HSMWorks which is virtually identical to Fusion on the CAM side.
    The secret to cavity work is that you run the roughing with a very small step up... my default is 0.005" and a very small radial DOC (a 1/8" cutter gets about a 0.0035" stepover max and I run an axial DOC as deep as I have flutes.
    With such gentle cutting comes the ability to rough very close to finish geometry SO LONG AS YOU SET YOUR TOLERANCE BAND AND SMOOTHING APPROPRIATELY AND DON'T TRY TO GO NUTSO ON YOUR FEEDRATE.
    80 IPM is about the max I trust my machine to execute without gouging at 0.005" stock allowance but my Minimill is a dinosaur from 2001 with no HSM and not much lookahead.

    Next, I like to run Garr Die-Mold cutters for finishing wherever possible because they are so nice and stiff.
    However with care you can run regular ball nose or bull nose cutters so long as you pick out the corners first so your chipload is as even as possible for the whole toolpath.
    Don't try to plunge into a corner even a little bit in P-20 with small cutters...you'll break them like popcorn.

    This often means a second adaptive roughing toolpath with a smaller cutter using a rest machining strategy...sometimes even a third roughing toolpath with an even smaller cutter.
    Adaptive is wonderful for this kind of milling...you can do some amazing shit with it, and I've pulled cavities off the mill I didn't think would ever work but worked just fine.

    For finishing Scallop is your friend wherever possible and you want to climb cut whenever you can with a small stepover.
    A 5/32" ballcutter with an 0.005" stepover makes a finish that's good enough that you see the individual flute marks and the dwells and gouges of direction reversal more than the scallop peaks when you look at it under the microscope, so there's no point in going with a finer stepover with this size range of cutter on a budget mill like a Minimill.
    As I emphasized before, you want your remaining stock to be as evenly distributed as possible before you start driving your finishing cutter over the surface.
    Occasionally I've played my finishing program up 0.001" and then run it again at final height, but the success of that depends on the part geometry.

    There are also some things specific to the molds for a Morgan or other lightweight press.
    The first is parallelism...you want to be as accurate as possible...0.002" out of parallel is super hard on the press because everything is so wimpy and you'll rack the shit out of the pillars if it's off that much.

    Ideally you will be within 0.0005" for the WHOLE STACK; easy on a surface grinder but hard on a mill.
    So whatever you do, mike the assembled mold and correct any deviation from parallel before you deliver the mold.
    Nobody gives a damn how the individual halves mike, but the overall must be very good.

    Second, molds for a Morgan press typically do not have leader pins, they rely on a tapered seat to locate the halves to each other.
    When you cut these seats, make one side nominal and then fit the second side by playing the program up 0.020" or so, then spot the halves together and feeler gauge the gap and finally play the program again at final height.
    When you do this you MUST be sure you're ONLY cutting the sidewalls and not the floor.
    The reason is obvious when you think about it.

    I always put a relief at the corner between wall and floor on both the male and the female side of the seat so I know I am clear in the corners and the locating is happening only on the tapered faces.
    Give the sidewalls 10 degrees per side and make the fit dead nuts so it blues off on both the sides and the parting faces, then whisker over the sidewalls with a 400 grit stone so it's not too tight when the mold is hot.
    It shouldn't stick at all when it's clamped and released but it shouldn't rattle either and the difference is tenths at 10 degrees.

    Last, the locating features on the undersides of the mold halves.
    For a loose mold, this is how you center the mold in the press so the sprue orifice is centered over the injection nozzle.
    Since Morgan molds are not commonly cooled, the features you thought were cooling ports might well be these location features.
    They need to be reasonably precise relative to one another...if I'm guessing correctly here, that's why they were toleranced by your customer.

    So you need to be sure you get them right and you only have one shot at it.
    Cut them undersized, interrogate them for position and then adjust location and cut them finished.

    Of course if I have guessed wrong, all of what I've just said doesn't apply, so find out if I've been bullshitting you and report back.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining
    Last edited by implmex; 10-21-2019 at 12:16 PM.

  7. #27
    Join Date
    Mar 2011
    Location
    Geneva Illinois USA
    Posts
    6,134
    Post Thanks / Like
    Likes (Given)
    2590
    Likes (Received)
    2379

    Default

    A lot of wisdom Marcus!

    Tom

  8. #28
    Join Date
    Jan 2018
    Country
    ALAND ISLANDS
    Posts
    66
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    8

    Default

    Yes Marcus, if you can't dazzle them with brillants baffle them with... well you know

    Sent from my SM-G960U using Tapatalk

  9. #29
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    2

    Default

    No NDA, but he did share that it was for manufacturing toy parts and that I make sure it doesn't go anywhere in that area. So while I'm sure most of us aren't involved with that, I'm still going to refrain from putting it out there for the whole internet. I'll DM the couple of gentleman that offered to give it a once over.

    I can come back and post any takeaways so I can maybe help someone else down the road.

  10. #30
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    2

    Default

    Marcus- Thank you for taking the time to write all that. As if all the mold-specific info wasn't gold enough, I learned things about my mill I didn't know either. Definitely archiving your post in my Onenote archives.

    And sorry, didn't see your post before I replied to the thread.

    I'm going to digest all that but to try and answer some of your questions:

    Quote Originally Posted by implmex View Post
    First, do you have your own seat of Fusion?
    Second do you know how to run it for 3D milling?
    Third, have you ever milled P-20 before?
    Yes, yes, and no. I've done other tool steels but not P20 in particular.

    Comments:

    Quote Originally Posted by implmex View Post
    Next topic, toolpaths and cutters:
    I run HSMWorks which is virtually identical to Fusion on the CAM side.
    The secret to cavity work is that you run the roughing with a very small step up... my default is 0.005" and a very small radial DOC (a 1/8" cutter gets about a 0.0035" stepover max and I run an axial DOC as deep as I have flutes.
    With such gentle cutting comes the ability to rough very close to finish geometry SO LONG AS YOU SET YOUR TOLERANCE BAND AND SMOOTHING APPROPRIATELY AND DON'T TRY TO GO NUTSO ON YOUR FEEDRATE.
    80 IPM is about the max I trust my machine to execute without gouging at 0.005" stock allowance but my Minimill is a dinosaur from 2001 with no HSM and not much lookahead.
    -I have a small carbide high feed mill from YG-1 for hard steels that I was considering using for the roughing op since they have strong cores. Is that something you would consider for this? Per your recommendation I'd get any corner features (most likely pencil toolpath,) and then step down in cutter diameters with REST toolpaths. I thought I could try to get a fine enough stepdown with the high feed that my stock to leave would be fairly consistent for the following REST ops. Then finish with .005" for scallop finishing. This is all best case without any running any +Z offset runs, or any of the good ideas you've shared for double checking, etc...

  11. #31
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,543
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1980

    Default

    Hi TheWolfOfWalmart:
    I tried to send my reply to you as a private message but it will not send (The message was too long to send with the PM utility)
    For all other readers, the OP sent me a link to his design and my response is to what I saw in his files, so here is a copy of that message:

    Hi TheWolfOfWalmart
    OK, so this is an insert for a standard mold and not a Morgan press kind of mold.
    That makes all of what I wrote about Morgan presses and their unique requirements interesting trivia but not relevant to what you need to do or consider.

    So here we go:
    Clearly the customer has a good grasp of what he wants and he obviously knows his turf, so your job is to make what he needs based on his drawing and his model and not second guess his design.
    The task as you correctly described, is actually pretty simple; there are really only a few things about it that can bite you.

    First, the drawing states that the insert will be preground but it is unclear whether the inserts will be ground to final size BEFORE you receive them or AFTER you have cut the cavities in them.
    This obviously is important for you to know.
    A common way for a mold maker to get the cavity halves to line up perfectly is to mill the cavities into oversized blocks and then to grind the outsides of the blocks to get the milled shapes into the position he wants them...it's a holdover from the days when grinding was much more accurate and predictable than milling, and a lot of toolmakers still do it that way because it allows several shots at getting it just right.
    So clarify that question first. (Typically moldmakers leave 0.005" grinding allowance on the outsides of the blocks and if you mike the blocks before you start cutting, you'll often be able to guess what the moldmaker intends, but do take the trouble to check with him before you assume.)

    Second, the complex water system...I've never seen it done that way before and I assume he intends to bolt another insert to the one he's shown you and needs to do this goofy design because he has no other room to place bolts and needs to compress an oring with the bolts.
    The counterbore you see is for that oring and the three little holes that surround the center tapped bore are to get the water past the bolt.
    It's a clever design, but so far as I can see, it's just for water, so there is nothing too fussy about it except for the finish at the bottom of the counterbore...it must be good or the oring will leak, and it must be the right depth: too shallow and the inserts can't be bolted together; too deep and the oring won't be compressed and the assembly will leak.

    A small tip; I'd be inclined to drill those small holes first, then cut the counterbore, then drill the cross hole or you risk breaking the small drills when they break through on the curved surface of the cross hole and if you do there's no easy way to get the broken drill back out.
    I can't see if the cross hole is a through hole or a blind one, but I'd consider drilling it undersize and then poking an 11/32" endmill partly down the bore followed by an 11/32" reamer to clean it up.
    It'll end up oversized by a few thou that way, but it'll make a nice clean hole that will accept the 1/8 NPT tap perfectly and it will make it look like that feature was made in a civilized country instead of a hack job by a savage in the bush.

    Moving on to the cavity: most of it is totally simple, but there is one area of concern and that is each end where the 0.02" radii are specified.
    You'll need to nibble these with a tiny cutter... a 1/32 4 flute ball mill will get into that corner, as will a 1 mm ball mill (just barely) but you'll need to either buy a necked down cutter or neck one down yourself.
    Once you've roughed the cavities with a 1/16" cutter within 0.001", pencil trace these corners in, moving from the open part of the cavity toward the corner and take it in several goes leaving stock of 0.001" in the corners too, before the cavity is finished.
    You can then use the same cutter to scallop the whole the cavity and it'll come out slicker than snot with no witness marks from cutter mismatch.

    You will have a scrawny little cutter hanging out a mile and it will flex and chatter and break off and drive you frickin' nuts unless you take it very carefully.
    Neck it down the absolute minimum necessary to clear the cavity sidewalls...0.010" too long will make a noticeable difference.
    Taper back the neckdown as you can...the goal is to have as strong a shank as you can and every bit helps.
    Model the shape of the cutter in Fusion and tangent mate it into the assembly so you can check for clearance.
    Get AB Tools to neck a few down for you if you can't find anything from Harvey Tools and don't have the means to neck down your own.
    Buy enough to be able to break a few.

    I personally would sinker EDM these, but you don't have one so you need to take the time to nibble it out gently on the mill instead.
    0.0005" to .001" stepover feels about right for this pencil trace operation and 0.0005" to 0.001" stepdown also feels about right.
    The main concern is that you never take a big bite with that cutter: at best you'll gouge the shit out of the sidewall as the cutter flexes under a big load, at worst you'll gouge it and snap off the cutter.
    This is a place where it might be worth it to make a trial run to prove your programming before you commit to the final blocks.

    Everything else is duck soup...simple programming and simple cutting.


    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining
    Last edited by implmex; 10-21-2019 at 02:10 PM.

  12. #32
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,543
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1980

    Default

    Oh yeah, while I'm at it...don't chamfer ANYTHING!!!
    Make it EXACTLY like the picture...some of the features don't matter but some do.
    You won't be able to tell which matter, and if you even just run a stone over it in the wrong place it'll be fucked up beyond recovery.

    Cheers

    Marcus

  13. Likes Philabuster, Greg White, Bob E liked this post
  14. #33
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,778
    Post Thanks / Like
    Likes (Given)
    10482
    Likes (Received)
    3203

    Default

    I don't do mold work, but I do often used necked tools. If you can't find what you need from Harvey or Helical (both great tools, though you do pay for it), these guys do necked cutters, and if you need something slightly different from what they've got on the shelf (like a longer neck, or say an .029"Ø instead of .0312"), they'll usually grind, coat, and ship it in 3 days, and just charge you the standard price instead of pricing it like a custom. Here's their 1.5x LOC 5x Reach micro endmills, you can peruse the other stuff to find exactly what you need S71 - Square Micro End Mills / 1.5x LOC / 5x Reach | MITGI

    No affiliation, just a happy customer, and they're not well known, so I figured I'd make you aware of them. Performance equal to Harvey, much less pricey. My opinion/experience only.

  15. Likes Philabuster, TheWolfOfWalmart liked this post
  16. #34
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,661
    Post Thanks / Like
    Likes (Given)
    1522
    Likes (Received)
    1738

    Default

    Quote Originally Posted by TeachMePlease View Post
    I don't do mold work, but I do often used necked tools. If you can't find what you need from Harvey or Helical (both great tools, though you do pay for it), these guys do necked cutters, and if you need something slightly different from what they've got on the shelf (like a longer neck, or say an .029"Ø instead of .0312"), they'll usually grind, coat, and ship it in 3 days, and just charge you the standard price instead of pricing it like a custom. Here's their 1.5x LOC 5x Reach micro endmills, you can peruse the other stuff to find exactly what you need S71 - Square Micro End Mills / 1.5x LOC / 5x Reach | MITGI

    No affiliation, just a happy customer, and they're not well known, so I figured I'd make you aware of them. Performance equal to Harvey, much less pricey. My opinion/experience only.
    FWIW, Harvey makes/sells odd sizes too. .023-.024-.025-.026 etc, in extended reach etc... Not that pricey (IMO) for a tool you need...

  17. Likes TheWolfOfWalmart liked this post
  18. #35
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    2

    Default

    I've been very happy with them as well. Did not know they would do customs so reasonably. Thanks for the tip

  19. #36
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    2

    Default

    Marcus- Thank you for looking that over and for your insightful post. A lot of info in there that is valuable outside of the context of this particular job.

    Taking all that into consideration, I sent the guy my quote. Not very hopeful that he'll bite, it came out to be a ludicrous amount of straight spindle time.

  20. #37
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,661
    Post Thanks / Like
    Likes (Given)
    1522
    Likes (Received)
    1738

    Default

    Quote Originally Posted by TheWolfOfWalmart View Post
    Marcus- Thank you for looking that over and for your insightful post. A lot of info in there that is valuable outside of the context of this particular job.

    Taking all that into consideration, I sent the guy my quote. Not very hopeful that he'll bite, it came out to be a ludicrous amount of straight spindle time.
    Hey, ya never know... I've done single pieces that were days of machining pre-heat treat, then post heat treat. I don't recall the hours, but I did one piece that started out of A2 (I think, it was tool steel) 7-7.5" thich by 22" square! Building a mold or die takes alot of components in general...

  21. #38
    Join Date
    Jul 2003
    Location
    Carson City, Nv. USA
    Posts
    902
    Post Thanks / Like
    Likes (Given)
    712
    Likes (Received)
    480

    Default

    You are so far out over your skis, that you have no idea as to how far.

  22. Likes TheWolfOfWalmart liked this post
  23. #39
    Join Date
    Mar 2011
    Location
    Geneva Illinois USA
    Posts
    6,134
    Post Thanks / Like
    Likes (Given)
    2590
    Likes (Received)
    2379

    Default

    Gotta start somewhere.

    Tom

  24. Likes TheWolfOfWalmart liked this post
  25. #40
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,543
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1980

    Default

    Hi All:
    Having had the advantage of seeing what was being quoted on, I believe this job was mostly about learning how to mill P-20 with a 1/32" ball cutter on a Minimill, and not about mold design or even about moldmaking.
    So long as the picture is followed without deviation, the OP's knowledge (or not) of the details of plastic injection molds will be immaterial to his success because he has just one specific thing to make and he has a good set of instructions on what he is expected to produce.

    This project is about..."don't question how much butter, just bake the fucking cake...here's the recipe".

    The whole trick is those damned corners.
    So here is what he's up against; picture two spheres stacked one on top of the other with a cylindrical neck joining them.
    Slice off the top and bottom of the stack, radius the corners 0.020" and then put a smaller cylindrical neck at each end.
    That describes the part.

    Now split a hot side and a cold side cavity from the part file...that's what you've got to mill.
    It's an ideal cavity to sinker EDM standing both inserts up with a 1" gap between them and running a spinning electrode between them, shifting over 1/2" to the hot side and then 1/2" to the cold side.
    Easy as pie to burn that way, and dead nuts accurate with a simple CNC turned electrode.
    Maybe a days' work all in, for a pair of cavities if you've got the goodies to do it efficiently.

    Milling them, I'd expect the time to be about double that for a cavity pair, and there might be a few more curse words that have to happen before all is done.
    But this is by no means "way outside the envelope crazy shit" it's still a pretty routine job if you've done this sort of milling with small cutters in prehard steel before.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •