Question Plastic machinability info

This is just my contribution for those of you that are embarrassed (like me) by the wide range of plastic materials today available.
Here below a selection of the "best" resources that I've found (after spending a lot of time on Google). You can use it to have a first overview of the "panorama".

General diagram of plastic machinability (note: Delrin = acetal):
Ease of Machining of Plastics

Another machinability list but with a huge amount of additional info (click the links on the left side):
Machinability of Plastics

When what above is not enough for you, then check also this:
Guide to Plastics Machining

Hope this helps!

My contribution here:

material = POM-C
milling bit = Carbide 2-Flute End Mills
rpm = 20000
feed rate = 400 mm/min (6.6 mm/s)
plunge rate = 90 mm/min (1.5 mm/s)
cut depth = 1.0 mm

I was comfortable with what above, that means ... very low rate of vibrations. Probably the depth of cut could be increased to 1.5 mm without problems but vibrations increases too. Nothing serious in any case, but I prefer to avoid it. I have plunged down in the material for 1 cm of depth.

I bought the milling bit by cnc-plus.de (code F-60-0104-60, price 24,00 Euro).

Tschuss!

Julius,

why did you choose 6mm? Do you have a lot of flat faces? Or is it because of the length?

For contoures I would rather use a 3 or 3.125 mm (1-flute) at same speeds. It's much less stress to the machine.

I do have only 6mm 4-flutes which I use for faces (to plan my vacuum table or all sorts of wood. (just have seen that I could use it also in Alu )

Everything else I do with 0.8mm-3.125 mm 1, 2 or diamond flute.

frankjoke wrote: why did you choose 6mm? Do you have a lot of flat faces? Or is it because of the length?

Hi, I have to carve some 50x45mm boxes in POM-C. I've thought that a 6mm-dia tool it's more rigid and I can cut more deep down into the material... I'm wrong?

Now I'm facing a problem when carving material deeply. My target is to mill down 19mm of material (!), apparently this cannot be done with the SC300.
The machine generates too many vibrations when going down more than 12-13mmm. In one case it has crashed the material (see photo below).
But I found a remedy: introducing some "horizontal steps" when milling down helps a lot about vibration-reduction. I've milled down to 19mm without big problems.
Drawback: you will not get a pocket with vertical walls




Today I will try to reduce greatly the feed rate to see if it helps.

As I understand, the structure of the Stepcraft is not so rigid. I mean... if you don't move your Z-position so far away from the "horizontal-bridge" of the portal, you can mill Kryptonite with no problems. But when you move down a lot, then the leverage (between the end-mill and the horizontal structure of the portal) increase drastically, this leads to big vibrations that will destroy the plastic material.

It's my analysis correct?

Decisevely, I have reduced feed rate and, even if not disappeared, vibrations are reduced. I see now no risk for breaking the material.

FOR CUTS MAX 19mm DEEP INTO THE MATERIAL:

material = POM-C
milling bit = Carbide 2-Flute End Mills
rpm = 20000
feed rate = 200 mm/min (3.3 mm/s)
plunge rate = 90 mm/min (1.5 mm/s)
cut depth = 1.0 mm

BUT YOU HAVE TO USE MY SELF-INVENTED "Top-Down Pyramid" TECHNIQUE






In the picture above first two levels of the pyramid are 7mm deep, last one is 5 mm deep.
Steps between levels are 1mm wide, this means that there is a border of 1mm running around every level. One millimeter provide enough room for free vibrations of the tool.

Hope it helps

Found some old tricks for POM milling in an older german thread.

1. Cut with an offset of 1/3 of the cutter diameter in a first run. After that do a final run without offset. Cutting surface will look much better then.

2. You can prepare a cutter to work better with POM. You´d simply leave a cutting edge of 2-3mm and file off some 10th mm of the rest of the cutting edge. To do that you can run the spindle and cut a 2-3mm hole into a piece of wood, letting the spindle run. Then take a diamond file and file off the part above from the running tool.

Hope I found the right words for this explaination.

Hi Julius!

The vibrations are defenitely not good, they are a sign that something is not right, but this could be also a bad spot in terms of spindle speed+feed and mechanical intereferences.

Try to change spindle speed on the fly up and down to have the best (most silent) 'sound'.

On the 6mm: It needs to move out twice as much material at the same time than a 3mm, and therefore generates at least twice as much stress, force, and so on. Of course, it could would be faster.

Yesterday I killed myself two 1mm mills, running before 3 month without any break. It was normal plywood and I did the same already 3 times before. I used then a diamond version instead the 2-flute and it worked well again, but I don't know why it happened. I will need to find out more about this as well!

BTW:
I think RPM is much too high for a 6mm cutter. The bigger the diameter, the higher the speed is on the cutting edge. Higher speeds result in higher temperatures. And POM is a plastic which should not get too hot. On one of your links given in the first post they mentioned the so called glass temperature. At this temperature the cutting behaviour changes to the bad.

When I cut POM I used a 2mm 2 flute at 20000rpm. So, for a 6mm cutter you can reduce speed a lot. From my gutt feeling I´d say something around 12000-15000 should do fine - if not less than that.

MagIO2 wrote: Hope I found the right words for this explaination.

I need some time to deeply understand what you wrote... but I will get it, I'm sure!

@Frank, @magio2

what you wrote is reasonable, absolutely. I've spent days (!) reading american CNC forums about POM machining, the mantra says:

- high speeds are unnecessary;
- calculate the chip-load per tooth
- take in account climb milling effects
- avoid machine resonance (a lot of diagrams about this)
- and... and... and..

Well, I've examinated a wide range of speeds for my 6mm cutter; from 7000 to 13000 rpm. For every speed I have combined it with three different feed rate and cut-deep of 1.5 or 2mm. A lot of tests!
Result was only one: frustration.
Always the same sound: rototot rototot rototot...

So I've done a reset of my mind; set the machine at the max rpm, lowered the cut-deep to 1mm and... it works! What I could say more?

I think that the main problem is that our machine is not rigid/stiff enough like the ones used in that american forums. Leaks in rigidity doesn't allow to make any optimization; sometimes the tooth hits the surface of the material where we want, sometimes it doesn't.. that's life! A vibrationg life!

IMHO, the best configuration is the Sherline-like one. I mean the one with a solid steel-column supporting the Z-axis and the table moving below of it.

In fact, the weakest point of our Stepcraft are the movements along the Y-axis. During my last (extreme) experiments I heard clearly the change of the sound when milling along the Y-axis. It's a clear signal that the leverage acting on the Z-axis is not supported by the machine. The bronze wheels mounted on top of the portal are perfect to contrast longitudinal forces, but their resistance to the transversal ones is close to zero... so when the Z-axis position is a little bit extended and you're milling deeply in the Y direction the leverage acting on the bronze wheels is great.
In Sherline-like machine the effect of this leverage on the Z-axis is close to zero. The unique deflection is the one of the tool itself and (maybe) the collar of the spindle.

(I'm not sure of what I wrote above, but please act like I was )

I`ve said it before, but the Operating Instructions state that you should work using milling cutters with a diameter of up to 3mm, so you might attempt something the machine wasn`t meant to do. It is a desktop router afterall.

On my machine the x axis is the first to start losing steps in case of a high load. Probably because of that smaller motor.

tikka wrote: I`ve said it before, but the Operating Instructions state that you should work using milling cutters with a diameter of up to 3mm, so you might attempt something the machine wasn`t meant to do. It is a desktop router afterall.

Well... in one of my old post Rory said that I could attempt to use big cutters with POM. I think that a 3mm-dia cutter will have more problems 'cause it is less stiff. The biggest collect that you can order by Stepcraft is 8mm (!)

Honestly 6mm cutter works quite well, but I will try to use my 1/8" milling bits and carve the same pocket to see what happens.

tikka wrote: On my machine the x axis is the first to start losing steps in case of a high load. Probably because of that smaller motor.

This is strange... really strange...

I used my 6mm 4flute today as well!

Had nothing else long enough to cut through 20mm hard wood.

You will see that my vakkum-table was actually not used with vacuum but with clamps.
The black rubber is to drill through (and avoid easy moves of the part).

I did 300mm/min (5mm/s), 1mm down and 12000 RPM in this hard wood.

A 6mm dual fluted cutter will remove twice as much materials and due to the increased material removal rate the machine will have to work harder - both the spindle and the machine.

router spindles have terrible torque at low RPM and are often air cooled.. direct drive of main shaft... so the lower RPM puts everything under pressure. OF course the lower RPM helps as we don't want "rubbing" where the cutter is spinning too fast and heating up. This results in poor results, lost work, broken cutters.

how can we improve this? Use a single flute instead of a double flute. A single flute halves the necessary feedrate at which rubbing will occur as we have only 1 flute - not 2. This is good as the STEPCRAFT is a "slow" router. We want to keep the spindle speeds up to get the max torque out of spindle and we also want to reduce rubbing.

The best solution - for plastic for example - use a single flute, max the spindle RPM, Machine with a feed of at least 1000mm/min and take shallow passes.

The shallow passes also helps as the STEPCRAFT is not a heavy stiff production router - so with a 6mm cutter there is a lot of leverage of the cutting tip over the machine.

Router are designed with spindles that move fast. So... The best strategy is to move the machine quickly and remove less materials, and if using plastic (and sometimes ali) use a single fluted cutter

for example - in a test we did recently - we were machining 0.5mm aluminium with the commercial routers on a vacuum table. The process worked so much better when we took only slivers of material off. 0.2mm per pass and moved at 3,500mm/min. with the spindle at 20,000RPM.

julius wrote: @Frank, @magio2

So I've done a reset of my mind; set the machine at the max rpm, lowered the cut-deep to 1mm and... it works! What I could say more?

perfect. Now try with singe fluted cutter and 0.5mm per pass and speed up the feed.

MagIO2 wrote: Found some old tricks for POM milling in an older german thread.

1. Cut with an offset of 1/3 of the cutter diameter in a first run. After that do a final run without offset. Cutting surface will look much better then.

exactly - its called a spring cut.

- Machine down in the steps of 0.5mm or 1mm or whatever you use... but leave a space of say 0.1 or 0.2mm from the final geometry. so there will be a faint line in the wall where the steps are each time.


- now machine down the full depth - so 20mm per pass - but now take the shaving (0.1 / 0.2mm) off the wall - this will give one clean face at the end.

watch here from 18 seconds you will see the final pass. Now - careful as the STEPPI is not a large mill and the cutter at full depth is risking over load. So only take a shaving off at a time.

Rory wrote: The best solution - for plastic for example - use a single flute, max the spindle RPM, Machine with a feed of at least 1000mm/min and take shallow passes.

Ok, trying with a single flute it's my next step. But... what the diameter of the bit should be? As I see, the Stepcraft works better with big diameters when you have to go deeply in the material.
Yesterday I made a test: I have returned back to a 3.175mm 2-flute end-mill:

rpm = 20.000
doc (depth of cut) = 1mm
feedrate = 3.3 mm/sec

A lot of noisy vibrations everywhere even, after one minute it starts to lose steps on the X-axis (!).
I remain of the same idea: for me nothing is better than a stiff tool (5mm-6mm dia)

The shallow passes also helps as the STEPCRAFT is not a heavy stiff production router - so with a 6mm cutter there is a lot of leverage of the cutting tip over the machine.

Rory wrote: T
exactly - its called a spring cut.

- Machine down in the steps of 0.5mm or 1mm or whatever you use... but leave a space of say 0.1 or 0.2mm from the final geometry. so there will be a faint line in the wall where the steps are each time.


- now machine down the full depth - so 20mm per pass - but now take the shaving (0.1 / 0.2mm) off the wall - this will give one clean face at the end.

Ok, I will try to leave just 0.1 or 0.2mm as steps of my top-down-pyramid and, after, apply a "spring cut".

In the meanwhile another record: using the "pyramid" technique I have milled 2,1cm deep into a POM-C block! Amazing! That was 3 steps with 7mm height (7x3=21mm) and 1mm of offset between the steps.
As final step I've erased slowly the steps of the pyramid to make the walls perfectly vertical. The finishing is not the best, I think the "spring cut" will work better

Rory wrote: router spindles have terrible torque at low RPM and are often air cooled..

---

Yes, I've got sensation of that. I reduced the rpm of my 2-flute/6mm-dia to 6.000 rpm and... after less than minute I broke the material. So it's better to keep our babies at high rpm.

Again, the idea of the single-flute + high rpm is really good IMO.

Noise and vibrations - drop the pass depth. try 0.25 as example? Its better do do this and run the machine quicker.

Let us know the results of the single flute. You can get single fluted cutters for plastics.

Rory wrote: Noise and vibrations - drop the pass depth. try 0.25 as example? Its better do do this and run the machine quicker.

I reduced just the DOC (Deep of Cut) from 1mm to .30mm and noise and vibrations are greatly reduced as you said.
Anyway, even with previous settings, they was at tolerable level. I think that 0.5mm is the best compromise between speed and vibrations.

For the ones of you that loves strong emotions: in the attached photo you can see a pocket 21mm deep (low quality, I made it with mein Handy.)

My last result as combination between the TODOP technique (Top Down Pyramid) and the Swing Cut one (by Rory).
I have slightly increased the DOC (Deep Of Cut) and the feedrate too. Very low vibrations, I'm satisfied.

TODOP params:

Material = POM-C
RPM = 20000
Feed rate = 250 mm/min
Plunge Rate = 90 mm/min
DOC = 0.5 mm

Swing Cut params:

Material = POM-C
RPM = 20000
Feed rate = 400 mm/min
Plunge Rate = 90 mm/min
DOC = 2 mm

IMPORTANT NOTE: above swing cut parameters works well only if you have to refine just the thin steps of the top-down pyramid (0.5 mm for every step, in my case) and produce a rectangular box. If you want to produce rounded corners for the box while applying the swing cut ten I strongly suggest to lower DOC and feed rate both.
For example, to round my outer box with 3mm-radius corners I had to lower Feed Rate to 300mm/sec and DOC to just 0.8 mm to avoid typical rrrrr-rrrrr-rrrrr vibrations.


Here below, a 2x2 cm experimental bulge. The height is 2,1 cm:




(don't take care if one side of the Pyramid seems slightly crashed, I didn't calculate the X-Y position of the box very well )

The steppie 300 is a great machine!!!