Hdpe milling frustration

How To Machining
1

Been fighting with vibrations and harmonics milling 1” hdpe.

I’ve got working holding issues cause vibration of the stock itself and I’ve got harmonic issues through the bit itself.

Have switched from a. 1/4” o flute to a 1/2” o flute. But harmonics are gone and I can take as large of a chip as I want if I wanted. Now I’m getting lifting of the stock but only during full depth finishing passes in inside curves taking .005-.010” passes.

I’m going to post some pictures and tool paths later.

My big question right now is. When cutting and inside curve. Does a larger diameter end mill have a more engagement with the stock than a smaller diameter end mills. Trying to figure out my stock lifting.

2

For roughing, bigger cutter = more forces. For a finishing pass that light light though, I wouldn’t expect much difference in forces between cutters of different diameters. Have you looked into “low helix” plastic cutting endmills? Particularly when you’ve cut most of your material away and don’t need to worry about chip evacuation, that might reduce the vertical forces on the stock. I know most O flutes aren’t that aggressive to begin with, but there might still be some benefit.

3 Likes
3

Back next to my computer. I had to walk away from the machine before it got to me. and decided to post then for some reason. I’m going to dump all the info I can to get it out there, hopefully its not too much

I have a .25" amana plastic specific o flute that I bought for this project 2 years ago. Customer has drug his feet back and forth due to the price and has finally made an order. I originally got all my tooth paths inline on my 3xxl with hdz and 2.2kw spindle. Now that I have a 5pro 4x4 with 2.2kw spindle I started with what I worked up to make the original proto type. Well that Didn’t work, Having horrible harmonics through the bit making roughing passes .25" deep at 100 ipm and 10k rpm, 6k to 24krpm didn’t make much difference. I actually broke that bit trying to get it sorted out.

I have now bought a 1/2" spetools o flute with a 1.25" flute length, and a 1/4 of flute with 1.5" flute length. I know the longer flute length is not helping my harmonics, especially with an o flute, but i need to be able to cut through this 1" and take a full depth finishing pass. I cant go into much detail on what these are, I can just say that surface finish in the concaved areas is crucial.

the 1/4" just showed 10 minutes ago. I do have some balance issues with the 1/2" bit Using the 1/2" I’ve been 6k-11k rpms .25" to .5" doc has been flawless, no harmonics issues what so ever, I even suppressed my roughing operation by accident and did a full depth slotting pass at 100 ipm and 12k rpm, finish was surprisingly good although the machine wasn’t happy.

The issue comes when I do my full length finishing pass due to the nature of this part i have a 1/4" hold down bolt on each end with 17" on center. from what i can tell the forces during my light finishing passes are enough to cause a harmonic movement in the plastic itself and if it lifts in one of the concaved areas it digs into the top edge ruining my finish. I am down to 50 ipm at 1100 rpm with the 1/2" bit for finishing pass. I don’t like that chip load but i can get buy with an air blaster.

Ideally I do not want to change bits for this operation. At this point of nearly given up on the jig as pictured. I cant risk 10 failing and i need to baby sit it anyway. I do have a vac table which means I need to make jigs to hold parts like these, which is nothing new to me I use front left corner as my zero with zero ontop of waste board. have bards screwed to the edge to locate on the vac plenum for consistency, I also bore 2 1/4" holes in the jig and engrave or write the absolute location of the holes to check alignment if needed. I use screw inserts in the 3/4" plywood for the hold down bolts, I also use a solid carbide drill to drill the hold down holds in the plastic, I’ve found that carbide drills have the least amount of runout.

part has two operations, one flat, the other vertical, I’ve got no issues slotting and drilling on the vertical.

part overview
part overview636×663 27.8 KB

jig has a 1/4" deep pocket to support the backside of the part all though I would love to be able to face the other side and have both sides unsupported

jig over view
jig over view1103×824 184 KB

.

stock is 1" thick , 18" long, and 1.625 wide as show below, this leaves me around 1/8" extra material just to make sure.

stock
stock1038×594 120 KB

Here is how I’ve been roughing, Haven’t had much of an issue there as long as i keep doc under 3/8 of an inch,

roughing
roughing1174×721 196 KB

finishing path is simple. the issue happens when entering the concaved areas and getting maximum engagement in the back of the arc.

finishing
finishing1144×675 159 KB

My current Idea is to machine a 3/8" to 1/2" aluminum brace that goes ontop of the material to help prevent it from lifting, Also hopes this gives me enough friction so I don’t need the support on the back side and can machine both edges to remove saw cut marks.

support
support931×728 113 KB

If you have made it this far through what I’m sure will come across as incoherent rambling, I’m sorry and thank you.

4

Not sure this would work but you can try. I use painters tape and super glue often. You can try a patch in the center to help hold down the material from lifting. Have not used HDPE so not sure if the tape would hold. Just make the patch on the spoilboard bigger than the spot on the material and be careful not to use too much super glue that would squeeze out. All of the painters tape does not have to have super glue to hold. Maybe an 8" square on the spoilboard and a 6 inch square on the material and put a 3" circle of circle glue so it does not spread out and glue itself to the material and/or spoilboard.

1 Like
5

Without having thought about it too much, it makes sense to me that a larger diameter tool will create more force in the arc.
I could see there being quite a bit of additional material at the apex of the arc, almost like rising forces in a corner but not quite the same…
In a perfect world, the diameter of the tool wouldn’t matter because you could keep the end mill tangent to the work surface at all times but we’ve got things like runout and material deformation to deal with.

As for the lifting, I’m not terribly surprised that it would lift in the center. At that point you are pulling up on a levered piece of plastic. Something deforming seems about right.
The bar/stiffener may help. I would recommend undersizing it a good bit just to reduce the chance of biting it with your finishing operation.

6

HDPE is pretty low surface energy so I wasn’t sure how well a general purpose adhesive would stick to it. Turns out I’ve got a block of natural hdpe and two types of painters tape sitting by me so it was easy to test…works surprisingly well!

I wouldn’t trust it as a primary source of hold down because as soon as it starts to peel at all, the whole strip comes right off. For a secondary additional bit of distributed holding force though, it’s worth a shot :slightly_smiling_face:

That said, the quickyest way to ruin surface finish is by getting tape/adhesive gummed up on a tool so be real careful about that if you do try it @quicky06

7

I really need/want to stay away from tape and glue. I’ll be making those 15-30 at a time to start with and that just seems miserable to deal with.

The stiffener I pictured is .020” smaller in every direction than the finishing pass would be. Which is plenty in my mind. Im going to have to find some flush counter sunk head boots for it. And make sure I can clear my cooler nut before order material. Either way will be Friday before I can play with it some more. Part of me wants to make one out of 1/8” baltic birch and see if it helps.

I’m tempted to rough with the 1/2” , leave 1/4” of stock then finish with the 1/4” taking relatively light and reducing pass depths. If I can get it right without the stiffener or with it out of wood I can make 10 at a time and the bit change becomes worthwhile.

Another option that I’m just now considering is one or two hold down bolts with a z shaped piece putting pressure on the middle of the part. Something to play with tomorrow.

8

Ignorant question. Would a down cut bit resolve it ? IDK is that is appropriate for HPDE.

9

Downcut tools are bad in plastics because they don’t evacuate chips, which results in re-cutting, which leads to chip welding, which usually brings about a disaster.

10

I knew it had to be a no brainer.

11

Without adding some workholding to the middle of the part, you’re not likely to get rid of vibrations. I would also recommend double sticky tape, but have it placed a little back from the cut. I use Nitto brand based on a recommendation from @wmoy and it works great. You don’t have to cover the entire part in it, and can just place it strategically. The other option would be to add some threaded inserts to the back of your fixture and use something like Essentials Clamps behind the cut.

I’ve cut a good amount of HDPE and on the S5Pro with a 2.2kw spindle, you should be able to double your feed rate safely. Play with the feed +/- in Carbide Motion and see if there is a feed/speed combo that reduces the harmonics.

I also echo that if a good finish is the priority, using a roughing strategy with the single flute, leaving 0.010"-0.020" of stock, then switching to a 2 flute to get a stronger tool and finer finish might help. With most of the material removed, more flutes is not as much of a hinderance. Also, I would recommend trying a 3/8" as I’ve found them to be the best combo of chip load and rigidity.

2 Likes
12

Which Nitto product do you use ? Thanks for the tip !

13

I’ve got some 3/8” thick t6061 bar stock coming.

Going to make my stiffener and see how that goes.

I will need to counter sink the hood down holes and run a counter sink bolt.

I’ll play with it this weekend.

1 Like
14

I use this version. Has a good balance of stick. :slight_smile:

Nitto 2x Tape

3 Likes
15

Well go my aluminum in. Side not @wmoy your feed rates frighten me. I’m a wood guy. Not an aluminum guy.

The top brace does exactly what I need it to. I put a piece of card stock in the middle to make sure it had pressure.

I’ve got a couple of bid requests out to make 10 of them with a surface grind to eliminate the need for the card stock.

Current settings are

75 ipm. 9k rpm. .25” doc with a .125” step over.

I’d love to double my feed rate but this Chipload works great and anything over 10k rpms and this bit vibrates crazy.

I don’t need the air for my roughing passes but I do for my finishing so I just leave it on.

5 Likes
16

Glad to hear you’ve got something that works for you! (Assuming you fixed that little crash in tool pathing at the end of the first video :wink:)

If this becomes a thing you need to do a bunch of or do often, there’s a lot of room to speed things up.
Of course it’s always a trade off in terms of time invested to optimize an operation. So if this works reliably for you as is, that’s still a big win.

Congrats on getting it across the finish line :checkered_flag:

17

Yeah I was hopping no one would notice that. I changed the height settings for my roughing but only changed the clearance height and not the feed height for the finishing path.

Chipped the tip of the bit a little. But I polished it out by putting a flat on the bottom. Not a huge deal. Plus it’s a cheap bit. Still cuts well.

I know there’s lots of room to speed up. This bit just has a horrible vibration preventing that from happening. 10k rpm is fine. 11k and it’s going to shake the machine apart. I’ve got to get this first round of parts out, so I’m going to be making them one at a time for now.

18

If you’re referring to the single flute 1/2"…I had the same experience. It was horribly imbalanced. It sits in the drawer barely used.

3 Likes
19

Yes. I can’t afford any more time tinkering with this right now. But I’m going to try to go back to a 1/4” or find a 3/8” after this. And see what the stiffener does with those.

2 Likes
20

Does the tool geometry look inherently unbalanced? If it’s a super low helix single flute then I could see that being the case and needing a big heavy spindle and head to keep it in place.

I use an 8mm O flute with a fairly good helix on it in HDPE, MDPE, Acrylic, Polycarbonate etc. and I can run that anywhere up to 24k RPM.