This means heat. It’s partially melting the material, and that is preventing the chip from exiting the cut.
Your speeds & feeds sound right. You’re running about ~600 sfm & 0.004" ipt which is right in the wheelhouse for acrylic. And it looks like others are getting good results with these numbers.
Perhaps the cutter isn’t as sharp as it could be? Try cutting the same path with a brand new tool.?
You could try doing a 0.0005" finish pass on each side of the slot, conventional cut at the fastest feedrate you can get away with to clean up the remaining chips.
Another option is try to get rid of the heat. Air blast? I might even try pouring a bead of water or alcohol/water mix on the material over the slot before cutting.
But honestly, as Liam suggested, if the quality of the cut is good, wrestle with your OCD & don’t worry about it.
I agree, the plexi chips are definitely heating because they stick like they’re melted together.
It’s a brand new bit. It’s the Amana 51411-K bit, which is intended for this type of cut… the 1/4” version was the same type of bit.
I appreciate your and liam’s advice of using auxiliary methods to clear the chips, which are certainly reasonable options… but that’s also not really the question I’m asking. I wasn’t just looking for a quick way out of this project, I’m hoping to learn more about cuts in general and adjust my settings. The more I learn about chip loads and heat during cutting I’ve come to understand that there’s a lot of depth of knowledge that I just don’t have in my dumb monkey brain yet.
The techniques you’ve suggested for clearing the chips… while they for sure are effective, don’t feel like the simplest possible method. I’m approaching this challenge as an engineering puzzle, and It feels to me that immediately jumping to using a blower or lubricant for these cuts is analogous to adding a pile of heat sinks to a circuitboard assembly without first doing everything possible to address all causes of excess heat. Sure it works, but could there be a more elegant solution worth exploring first?
My thought is that the solution could be a slightly adjusted feed rate, or depth of cut…I could certainly experiment for hours, wasting time and material, to learn what I’m hoping to learn, but was hoping for this specific type of guidance.
And I’m willing to accept that perhaps the answer IS, simply… “No, Jon. There is no way to dial this in”, because the general consensus from experts is that acrylic will ALWAYS do this 100% of the time due to static charge.
But if that’s the case, that must also mean I’m already getting the most perfect cut possible already and that my speed and feeds aren’t simply in the ballpark… they’re already perfect and I can’t do any better.
I’m just having a hard time believing that to be the case. I’m certainly not that good. Also, I’m obviously getting heat so something about my cut settings is probably not ideal.
Anyway - so far, no has said that it’s not possible to get a clean cut, only that it’s not worth the time… but mastering the skill is worth the time IMO. Sorry if that seems OCD, but i like to understand why things are happening so I can do better at it in the future.
I’ve seen videos & pics of guys getting really nice cuts on acrylic with no melting, so I know it’s possible.
Generally, when the problem is heat conventional wisdom says slow down the spindle, and/or speed up the feedrate. I suspect you can’t slow the spindle any more, so upping the feed is all that’s left.
Did you try with a smaller DOC? Less surface area would logically mean less heat.
I can’t imagine the paper would cause much heat, but what about the adhesive? It could gum up on the flute & add to friction??? Try the cut on a piece with the paper removed, maybe.
Apologies if the “OCD” comment offended. I have it too! It was a ‘cheeky’ comment.
“We’re all in this together. Keep your stick on the ice.”
I cut cast acrylic around 125in/min on my 3HDZ. The chips stick, but definitely don’t look as melty as yours.
What machine are you running? Regardless, feed faster. Adjust the depth of cut to where you feel comfortable.
I cut a lot of acrylic on the table saw as well… Sticks to everything.
No offense was taken at all Tod. I appreciate the advice you’ve given.
I’m realizing, after the initial replies, that I buried the lead of my original intent for this thread, which was essentially: “what are the order of steps you take to dial thr he cleanest chip-clearing cut on new material”. You’ve given me some good guidance, thank you!
I thought of something else.
I don’t use any coolant or forced air, but I have noticed a difference with the air temperature. Cold acrylic in cold air evacuates chips easier than room temperature acrylic warm air.
Oh that’s interesting, I’m glad you mentioned it. Not a factor this time around as I’m northern hemisphere and it’s been plenty cold in my garage lately… but will keep this tip in mind when I’m cutting plastics in the summer heat. Thank you for that
My garage is plenty cold enough in Ohio. Except for every other day when it’s hot enough to melt acrylic. Sometimes we go from below freezing to melting and back within a few hours. I’m sure it’s the same over there Wayne!
It’s probably worth considering that the other parameters of the cut, rather than being a heatsink bodge after the fact are rather inherent properties of the process.
Feed rate, DoC, WoC, cutter RPM are four variables in a much larger set which control what is happening during the cut. If we attempt to find an ‘optimum’ point in the space for just these four parameters we have found a set of parameters which work, given some other set of unknown parameters which may or may not change between now and the next cut and when they do change, we won’t know that they did, or how to adjust our known parameters to account for this.
Other key elements in this sort of cut, which all take part in influencing the overall observed performance include
Composition of the acrylic, coarsely whether it is cast or extruded, these behave quite differently
Local air conditions, as Neil pointed out temperature which affects the behaviour of the acrylic at the edge of the cutter, this is a huge parameter, acrylic starts to go goopy at a pretty low temperature ( I think about 80C but Google it )
A related variable, humidity ratio which affects the rate of charge leakage over the surfaces and in the air, impacting static charge buildup
Geometry of the cutter, not just diameter but the helix angle, sharpness of the edge, the face and relief angles of the edge etc. For example, an uncoated cutter will likely be sharper, because it doesn’t have a coating to round over the edge
Rigidity of the machine (which varies with X, Y position on a Shapeoko) impacting how the cutter meets the material, whether resonances build up etc. This applies to the workholding as well as the machine
Whether the dust extraction is effectively scavenging the slot the cut is in or waiting for chips to be thrown out by the cutter, the geometry of the dust shoe, proximity to the surface, flow volume at whatever pressure drop you have in the extraction system all impact this, dust shoe on/off is not a particularly useful parameter here. Also, the dust boot will likely perform quite differently dependent upon the direction of the cut
Related, an air blast to cool and purge the cut slot of chips, keeping the cutter cool, workpiece cool and force evacuating chips trying to hang around and melt
Lubricants and coolants, many coolants are also partially conductive thus reducing static charge attraction, they also reduce friction between the cutter and workpiece, as well as cooling the workpiece, cutter and chips
I’d suggest that options to reduce the static charge, keep the cut cooler, blast chips out of the slot etc. are all known key input parameters to impact the chip melting and stringing behaviour you’re seeing, they’re also much more likely to improve the performance in a reliable way than changing your already pretty sensible feeds and speeds. If what you’re after is to search the solution space, it’s worth trying the other levers as well as the four that you can change in CAM.
I forgot to mention, looking at the chips is just as informative as looking at the cut. If you really want to see what’s going on try emptying your extraction and then checking the chips you get on a new cut.
It’s a bit like being a vet on a farm but it works
I don’t have the words how much I appreciate your post, Liam. Love the way you’ve explained this. Sincerest thanks.
If you don’t mind a couple follow ups about a couple of the variables you mention?:
The acrylic is extruded. Cast is just too expensive for my silly projects. Should I be taking steps to adjust for this? Does extruded prefer any specific settings?
The humidity & temperature variables,
I’m curious about how different materials generally react on the +/- scale… do you find that most materials react similarly, relative to whether the temperature/humidity is higher or lower than that material’s ideal working conditions, or is it starkly opposite for different materials? Like - do PVC, VC, and MDF for example, all exhibit similar changes at higher/lower temp/humid (even if at different overall temp/humidity ranges)? I’m not cutting anything particularly exotic, really just plywood, MDF, and acrylic.
And if it is relatively similar at different scales, - is there a similar relation to changes in speeds/feeds that you would make to accommodate?
(Sorry I feel like I’m struggling to clarify this question, let me know if it doesn’t make sense)
And on a related tangent… I have a project coming up that will be using some high-gloss Gizir boards - this is a 3/4” mdf sheet double-sided with a thick layer of gloss black pvc and a peel coat. I’ll do test cuts to make sure I’m not going to melt the pvc while attempting to keep the channel clear of dust… but can I ask how you’d approach a combination material like this?
Well first off, don’t mistake me for an expert, I am learning just enough to understand how much I don’t know.
Regarding the acrylic, my understanding is that extruded has built in stresses and other issues, similar to how rolled metals differ from cast and stress relieved metals. There’s some useful discussion here
Extruded is more like chewing gum and is just going to be trickier to machine without stringing, if your current cuts are leaving a decent finish after you scrape off the stringy stuff, I would stay close to those settings, having to do a little deburring or finishing is not unusual.
The stringing is due to material heating in contact with the cutter, what this doesn’t tell us is which of the many causes are present in this particular instance though
Cutter surface speed (RPM and diameter) too high imparting too much heat at the edge (more of a problem with metals)
Cutter feed rate too low, hanging around to heat up the stock locally (poor thermal conductivity in plastics makes this worse)
Chip evacuation poor due to low helix cutter, narrow slot or other mechanical constraint
Chip evacuation poor due to poor extraction (suction or air blast)
Chip evacuation poor due to static charge buildup (plastics)
Cut would prefer to be done slower overall with a conductive lubricant…
It’s possible to make up for some of these by changing others, e.g. you could try reducing the RPM and the DoC together with the same feed rate to reduce heating.
You could also try one of the anti-static sprays that are sold for ironing and similar uses to address static build up on the workpiece, properly grounding your dust extraction is also a good start if you’re going to do a lot of plastics. Remember you can’t ground an insulator, but you can accidentally make a capacitor
Regarding humidity, it is very dependent upon the material.
Wood changes dimension with water content and this combines with pre-existing stresses in the wood to make it warp and curl as it’s cut, or soon after it’s cut.
For plastics the humidity issue is about static charge dissipation, the humidity ratio (not relative humidity) is understood to be the dominant factor in allowing static charge to build up vs. bleeding it away.
I personally wouldn’t try to compensate for humidity with feeds or speeds (I may well be wrong for wood here). In plastics I’d rather deal with the static buildup than try to compensate with RPM.
There are some excellent charts and resources out there which explain how surface speed of the cutting face impacts the temperature of the cut as it’s happening and why certain RPMs are recommended for a given cutter diameter in metals and plastics, reading up on these effects starts to explain why some speeds are just ‘no’, where coolants are required to stay in the effective window where neither the workpiece nor the tool are destroyed etc.
It’s not a simple matter of cooler is better, HSS works by having tools which stay hard at temperatures where the workpiece has started to soften for example.
For hardwood, plywood and MDF, I try to store the wood somewhere reasonably dry and let it adjust to local conditions before feeding it to the CNC. Birch ply has been the least temperamental for me, followed by MDF which doesn’t like extremes of humidity and hardwoods like Sapele which wait for me to turn my back for 10 seconds and banana. Given the frequency with which I am caught out, I clearly know almost nothing about wood and humidity…
PVC is IMHO, unpleasant, if you let it get too hot (or cut it with a laser) it goes black and gives off Chlorine gas which is not good for your health, or tooling. I have also found the static buildup on PVC to mean that the chips stick like termites to everything, even with dust extraction on. It is however, reasonably soft and I’ve had decent cuts in it running larger O flute cutters and mid-RPM and high feed rates.
For the combo PVC and MDF I’d probably try a reasonably large cutter 1/4" min, preferably 8mm with a good upcut helix to rough through the MDF. MDF blunts everything it touches so this cutter will only be good for roughing pretty soon. The better you can get MDF abrasive fluff out of the cut the longer the carbide will last. The trick will be not cracking or chipping out the surface plastics, or rather figuring out enough stock to leave on the roughing cut.
I’d probably then come back with a decent quality compression cutter at full depth and small (say 0.25 to 0.5mm) stepover and high RPM & feed rate to clean up the edge. The less you have to take off with this good cutter the longer it will stay good. I’m not sure that a plastics cutter would last very long in MDF. It might be worth asking the folks at Precisebits or another specialist if there’s a good combo cutter for this material.
I would definitely experiment with some offcuts first though in this mixed material.
Helps a ton, Liam. Expert or not, your experience is greater than mine and certainly valuable to me and others. I appreciate that you took the time to share in detail. If not comfortable with the title of “Expert”, consider “Teacher”, a far nobler title anyway.
I have lots to digest and follow-up upon, but you’ve helped me get a much more balanced and rounded understanding than I had 24 hours ago. Exactly what I had hoped for. Thank you again!!
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
Part of the problem with extruded is not just the internal stress (as mentioned previously) but that it uses a different recipe to actually lower the melting point (this is why they use extruded for thermal forming and it flame polishes better). The combination of the low melting point with higher internal stress makes it almost impossible to cut perfectly, without VERY material specific tooling (think “extrude acrylic cutter” not “plastic cutter”) or other equipment (air, vortex coolers, etc). Otherwise you are always either shattering the stressed material or partially melting it.
Keep in mind for the following that this is a tiny soft media tool. I’m intentionally trying to keep this vague due to bias issues and I don’t want anyone trying to use these numbers for anything other than the plastic comparison. To give you an idea I ran the same tooling from the same batch in some extruded and cast acrylic for testing. My test increased by 0.000125" (0.0032mm) chipload at each step. The extruded had a “tolerant” cut at one step 0.002" (0.051mm) chipload. The worst part of this is that, in our experience, even the same material from the same supplier might not run at that chipload again. This is due to the changes in processing of the plastic even with the same recipe. The cast material had a range of good cuts from 0.00275”-0.00325” (0.067mm - 0.083mm) (6 steps).
The geometry is where you can potentially get much better results in the material but cutter price starts to climb with extremely specific cutters. You can get a lot closer with plastic or soft media cutters as they have higher rake, different helix angles (lower for less “pull on the material, higher for more sear), more flute volume (places to hold chips in the flute), and relief to keep as little of the tool from touching the material. All of those things cost you in other areas though (tool strength, chip clearing, more stress to material, machine time, etc). So it’s always a fight between the economy of scale and the best tool for the application.
Yeah, coated tools in general I don’t like to recommend for plastics. It depends on the plastic, but you are always going to be dealing with a thicker edge slamming into the material (you coat the WHOLE tool). The advantage is less wear and possibly a smoother surface depending on the grinding wheels and coating used.
Are you sure this is PVC? Most of the stuff I looked at on their site is melamine, PET, or acrylic. The ultra high gloss is listed as “foil” on melamine.
Liam already got most of this. Basically a bigger upcut cutter for profile with a high speed clean up (not personally a fan of compressions but they are an option with pros/cons). There are a couple other specifics for multi material with deflection limited machining I’ll add though.
Won’t comment too much on the specialist tooling as again I’m bias. But it is possible with very high grades of carbide to make cutters that are both more aggressive and last. The blanks and processing material are more expensive though in addition to increased grinding time.
The first problem is that you have to find a feed and speed range that’s at least cutting both. Most likely it won’t be ideal for at least one though. Switching in this case to more aggressive tooling can help as they are both soft media. That will reduce the cutting force and get a “thinner” edge giving you a wider range at the cost of tool strength.
Even after accounting for that though you have 2 different materials with 2 different strengths changing the deflection. So once you are cutting anything but matching material(s) it will deflect more or less than before based on the strength of the different materials. That will end up slicing a very small amount off either the conventional or the climb side of the cut. This can leave a very poor cut or in the case of some plastics, melt it.
You can reduce the above effect by limiting deflection (shallower pass, less chipload) but you need to still keep it inside of the material range which is already limited by 2 different materials. In an ideal world we would cut it in a single pass keeping the load on the tool and machine the same throughout the cut. But we all have to deal with the limits of the tooling, machine, and materials.
Hope that’s useful. If there’s anything I can help with or expand on let me know.
That’s great John, I always have to read your posts at least twice to spot the things I didn’t know, then the ones I didn’t know that I didn’t know
I’d be interested in what the downsides are on the compression cutters if you have time. I can guess that shoving chips together to the middle of the material is probably not optimal but is this bad when you have an open side cut as opposed to slotting?
Thank you John, i very much appreciate your detailed answer. Much of what you said, admittedly, is over my head right now… but between yours, and liam’s responses I look forward to coming back to this thread in the future when I have a better frame of reference for the concepts that you’ve shared with me.
For the UHG Gizir board, I’m not 100% confident about the composition of the PVC specifically, but they call it a PVC/PET sheet on MDF. It’s definitely not foil or melamine. They do have other products in this line that have Mel or foil but this is the UHG in black.
Eyeballing the board, it’s about 1/32 thickness of whatever the blend of PVC/PET is that they use, on an MDF core. I wasn’t real excited about using a compression bit on MDF… I was originally gonna try for the whole thing with a single upcut, but then I’m thinking I’d just cut through the top layer with a straight bit, and then just take the rest of the MDF and the bottom layer with an upcut. I’d like to avoid an extra tool change for a third cut at the bottom. The good news is that only one side is the appearance face for my project, so I should be able to plan my cuts so If one of the faces isn’t quite as nice, I should be able to face it towards the inside.
You mention more aggressive tooling to balance the differences in material - can you give me a specific example of that recommendation? Is there a certain type of bit that I should be looking at? If you’re not comfortable with an open recommendation due to perceived bias, please feel free to direct message me. Thanks!
Not quite sure if that’s a failure or success on my part but I’ll file it in the Pro side for now.
Short version is that there’s rarely times that I find it’s necessary with proper feeds and speeds. Although, if those can’t be reached or maintained that would be a good reason to use one as a clean up where needed.
You’re right though that most of the problems are related to slotting (which is what they seem to mostly be used for). If you have an open side than most of the down sides are cutting force and geometry. They also tend to be more easy to break at the transition both from the meeting of the 2 cut directions and that most of the time more core has to be removed from the tool where they meet. The other option is to have an overlapping flute which is going to mess with chipload at that point. Add on cost and variations possibly needed for the transition point and it starts to leave a bad taste in my mouth.
No problem. Hopefully it’s useful either now or later. I might need to work more on the understandable part though…
PVC/PET mix should be a bit easier to cut in combination as it shouldn’t require quite as high of a chipload than straight PVC.
Assuming you are willing to deal with the multiple steps for the coding you could use just a single tool and modify you chipload and cutting depth per material.
I wouldn’t use a straight flute unless I had to as it’s the highest cutting force of pretty much and geometry. The issue is that unlike a upcut or downcut you are engaging the entire flute at the same time. This causes a very high sharp load to the machine and tool.
I’ll shoot you some specifics tomorrow. For everyone else though the basic things to look for are a higher rake, thinner edge and depending on the weakest material potentially a higher/lower helix. You also want a cutter the has relief and drop to keep only smallest part of the leading edge involved with the material. That last one does cost strength and potentially tool life though. If it’s someone you trust dealing with these kinds of cutters will usually be label for that specific material use. e.g. “soft media cutter”, “plastic cutter”, etc. Not listed as can cut it but that it’s designed for that material.
I did post some on geometry with some examples here Best practice for tiny endmills - #15 by TDA. Might help to understanding some of it. Although it’s in a completely different context. If I can get some time in the next couple days I’ll try to layout the basics in something more approaching english.
