Endmill failure or wrong feeds and speeds?
Hi,
I'm trying to pocket into 40mm oak to make a key tray. My first attempt worked fine and then I did a redesign and when cutting the bit failed. I was filming the cutting so I thought I would share it with you to get opinions on what went wrong.
My thoughts are it was a mildly blunt cheap old endmill. I think the feeds and speeds were correct for the size of the endmill just not the quality of the endmill.
These are my setting
Feed rate 4000mm/min
Spindle Speed 18000 r.p.m.
Pass depth 5.96mm
stepover 40%
This is the endmill
https://www.screwfix.com/p/erbauer-s...B&gclsrc=aw.ds
And here is the video to see what you make of it.
https://youtu.be/aPvKfQkM1Eo
My thought are should I buy a new cheap endmill of the same type and reduce the feed rate a bit and try again or buy a more expensive endmill?
Regards,
Oli
2 Attachment(s)
Re: Endmill failure or wrong feeds and speeds?
Re: Endmill failure or wrong feeds and speeds?
I've not looked at the video yet but I can tell you right away the cheap cutters from screwfix etc are exactly that - cheap!
I have used pretty much all the brands in this category and all of them dont last at all and generally snap/fail exactly like yours have. This includes the Trend branded ones (green craft pro) and the black "pro" range, the Trend cutters being somewhat "better" at lasting but still not good enough for what we do with these machines.
So why did this happen and what can we do about it?
The cutters mentioned above are TCT (tungsten carbide tipped) the Trend cutting blades in the black versions are better because the whole cutting blade/edge are made from carbide rather than only "tipped", however that's where the carbide stops and hence why they can suffer the same fate when pushed on a cnc machine.
You need to source solid carbide cutters for cnc work, you can find them available all over the Internet from different places.
Years ago solid carbide cutters where very expensive and even more so when you started looking at the big boy brand names etc, you couldn't really get them in small quantities "cheap" like you can now and in abundance.
The market has changed, thank you China!
So with that in mind, have a look on ebay, amazon etc at what is available, pic a supplier and see how their cutters fair.
If you can wait for items to come from China then Aliexpress is your best bet, again its a minefield on what brands/suppliers you order from but generally they are all on par with each other in terms of quality, BUT like everything there will be some rubbish out there too :hypnotysed:
So if you don't want to pay £££ for cutters and can wait I'll give you the link to the brand I use, I have a draw full of their basic range of cutters (solid carbide no fancy coating) and they have been fantastic in everyday use in wood, for about 18 months I have been using these cutters so can definitely vouch for their longevity, the only breakages have been from user (me) error.
Quality control.
So they are cheap, that means they are not going to be exactly on the money when it comes to sizes, however the brand I'm linking below are very close, my findings are that shank diameters seem to be spot on, lengths can be off by +/- 1-2mm (usually on the flute lengths) however flute major diameters are almost always slightly under size, my conclusion is that they produce the cutters as blanks then grind the cutting flutes (obviously) but dont seem to have allowed enough material for grinding the flutes in and for them to remain on spec, however that's ok and to be expected at these price points...
If you know, you know
When you buy any cutter, from any source, from any brand and at any price - you should ALWAYS check the dimensions of each cutter yourself. This is standard practice and like i say - no matter how much you pay for a single cutter, measure them all, number them and add them to your tool library/inventory separately with their own individual specs.
Link: XCAN 1pc 4mm/6mm Shank 2 Flute Straight End Mill Carbide CNC Router Bit Engraving Bit Straight Slot Milling Cutter for Wood
I've linked you directly to the 2 flute straight cutters, straight flute generally gives the best edge finish with an emphasis on slotting operations, for real wood, plywood and/or laminates where the top/face edge needs to be great (sharp/chrisp), go with a down cut type flute, this will help stop splintering.
Hope this helps :encouragement:
Re: Endmill failure or wrong feeds and speeds?
Next we should probably look at chip load and the relationship it has with speeds and feeds...?
Your speeds and feeds are to high for those cutters at that DOC...wow just started the video and straight away you can hear its all abit crazy, have a listen yourself Oli. I know it's hard when you first get going and dont have anything to compare to...
2 Attachment(s)
Re: Endmill failure or wrong feeds and speeds?
Some sound advice there Lee thanks for taking the time to make this response. Prior to starting the cut shown in the video I made a similar piece with all the same settings, F&S, DOC etc and wood from the same batch. The first run appeared to go absolutely fine with a good finish. So I did a new design and decided to record the cutting. The instant the cutter started it sounded wrong and I almost hit the reset button but for some reason left it going. The endmill appeared to resonate at a different tone.
So for the following, I used the guide on the Renne tools website https://www.rennietool.co.uk/blogs/n...eeds-and-feeds.
What made me approximate the depth of the cut was using the rule of thumb of half the cutter diameter. Which doesn't make sense to me the bigger a cutter gets. Then to come up with the feed rate I calculated what the minimum feed rate is based on their table playing it safe with the lowest values.
1/2 inch endmill in Hardwood = Chip Load 0.483 * 18000 RPM * 2 gives a feed rate of 17388mm/min 6mm DOC.
So the thinking was that a 4000mm / min would be no problem for even a poor-quality bit. I'll get a better quality solid carbide bit on order, as you say it's a waste of time with the cheap bits like I used. I'm just a bit nervous about coming up with the starting feeds, speeds and DOC. I'm wondering how you would approach F&S and DOC for a 1/2 " bit. Have I gone about it the right way but just used the wrong endmill?
I since finished off the project I was making using a 6mm solid carbide endmill and managed to recover the bit of wood thankfully.
Attachment 31302
Attachment 31303
Re: Endmill failure or wrong feeds and speeds?
Quote:
Originally Posted by
CNCOlly
Hi,
I'm trying to pocket into 40mm oak to make a key tray. My first attempt worked fine and then I did a redesign and when cutting the bit failed. I was filming the cutting so I thought I would share it with you to get opinions on what went wrong.
My thoughts are it was a mildly blunt cheap old endmill. I think the feeds and speeds were correct for the size of the endmill just not the quality of the endmill.
These are my setting
Feed rate 4000mm/min
Spindle Speed 18000 r.p.m.
Pass depth 5.96mm
stepover 40%
This is the endmill
https://www.screwfix.com/p/erbauer-s...B&gclsrc=aw.ds
And here is the video to see what you make of it.
https://youtu.be/aPvKfQkM1Eo
My thought are should I buy a new cheap endmill of the same type and reduce the feed rate a bit and try again or buy a more expensive endmill?
Regards,
Oli
Sounds like a lot of chatter with the cutter. What kind of spindle motor/router were you using ? Could be the routers not running true. Your ears are normally good indicators of how well things are running and tha cutter really sounded like it was struggling.
cheers
Andrew
Re: Endmill failure or wrong feeds and speeds?
Quote:
Originally Posted by
the great waldo
Sounds like a lot of chatter with the cutter. What kind of spindle motor/router were you using ? Could be the routers not running true. Your ears are normally good indicators of how well things are running and tha cutter really sounded like it was struggling.
cheers
Andrew
Hi Andrew,
It's a 2.2kw spindle. I think the chatter was a damaged bit from the first part I made using this cutting profile.
Here is a video of using the 6mm carbide downcut to recover the project. All appears well to me, see what you think.
https://youtu.be/eU9vK5n5jV4
Oli
Re: Endmill failure or wrong feeds and speeds?
Hi Oli
Sounds better. I would use as high speed as possible on the spindle with a 6 mm cutter with not too heavy a chip load. I always use my ears as a guide to how things are cutting.
Cheers
Andrew
Re: Endmill failure or wrong feeds and speeds?
Quote:
Originally Posted by
CNCOlly
Some sound advice there Lee thanks for taking the time to make this response.
No problem your welcome and welcome to the forum!
Quote:
Originally Posted by
CNCOlly
The instant the cutter started it sounded wrong and I almost hit the reset button but for some reason left it going. The endmill appeared to resonate at a different tone.
Yea, my guess is the first job weakened the cutter, the second job killed it...you cant rely on those cutters, not if you want to do it properly with cnc :)
Quote:
Originally Posted by
CNCOlly
What made me approximate the depth of the cut was using the rule of thumb of half the cutter diameter. Which doesn't make sense to me the bigger a cutter gets. Then to come up with the feed rate I calculated what the minimum feed rate is based on their table playing it safe with the lowest values.
Ok scrap that idea about half the cutter diameter, the general consensus is you should aim/start with a DOC that is equal to the cutter diameter, this is CNC machining so we should be looking for the most efficient cycle times, that result in the best possible surface finish etc. So, from the starting point of a DOC equal to the cutter diameter, we can go north or south of this depth depending on the situation (efficiency, surface finish etc).
The problem I've noticed with the various "speeds and feeds charts" dotted about is they don't seem to emphasise enough on a few things in my opinion.
I mean the Rennie page suggests:
Quote:
The recommended chip load & feed rate data provided below is a recommended starting point and may not accommodate all circumstances.
Ok, so what dose that actually mean?
Well firstly, it should be assumed that any of the charts provided by tool manufactures ONLY really cover the cutters they provide, when you start going to "branded" tooling, these charts are helpful BUT they are ONLY jump off points to get you in the right ballpark.
When they produced these charts, they did so on a different machine and under different circumstances to our own, so with that in mind everything should be treated as relative, its ok though because some of the fun is exploring and finding the sweet spot for our own circumstances.
The Rennie page didn't do to bad a job when they said:
Quote:
As a rough rule of thumb we usually advise the depth of cut as 1 x cutting diameter. However, in some circumstances a smaller or larger depth of cut may be optimal.
Always start out at the lower feed rate and work your way up from there until optimal cutting conditions and speed is acquired.
So really all I would advise anyone to do, is use these charts to get an approximation of the chip size for the material you want to machine, the rest is going to change and be different for everyone.
Rennie also state
Quote:
We would recommend running at 18,000 RPM for most single, 2 flute and 3 flutes up OR down cut router bits
I would say this is ok to get started with and quite a few seem to suggest 18K for the RPM, maybe its a good general spindle speed with plenty of torque for most feeds in lots of different materials, its not for everything though.
What they didnt say:
Spindle speed (RPM) is BAD for the longevity of cutters, End Mills, Router Bits etc.
When metal gets hot it also turns soft and this is no different for our cutters, to much spindle speed can generate heat in the tool and this will just make it blunt sooner. If you slow down the spindle speed it will give better tool life, when you find the right sweet spot and the perfect chips are coming off the material, make a note of the feeds and speeds, do the maths so you've got the magic chip size available for the circumstances/material, then you can start tweaking the spindle speed down adjusting the feed rate as you go in order to maintain the correct chip size you know works best for you. Keep in mind then that lowering the spindle rpm is better than reducing the feed rate.
Keep an eye out for the feed rate becoming to slow, we don't want the cutter to rub, get hot and then soft (tool life) we're looking for chips not dust!
Quote:
Originally Posted by
CNCOlly
1/2 inch endmill in Hardwood = Chip Load 0.483 * 18000 RPM * 2 gives a feed rate of 17388mm/min 6mm DOC.
A chip size of 0.483, a feed rate of 17,388mm/min with a 6mm DOC.
See the problem is, when you start going up in cutter diameter, the numbers want you start running your feed rates at some CRAZY speeds in order to maintain that magic chip size we love so much, when in reality, are those feed rates even viable. My comments are not so much aimed at the 17,388mm/min here but that feed rate should be observed, when you start getting up there in the feed rates, things like tool deflection start becoming a concern, what's the length of the tool below the holder, can we do those feeds with that depth of cut with a tool this size, is our machine even ridged enough, will accuracy be effected. Food for thought that's all.
Quote:
Originally Posted by
CNCOlly
So the thinking was that a 4000mm / min would be no problem for even a poor-quality bit. I'm just a bit nervous about coming up with the starting feeds, speeds and DOC. I'm wondering how you would approach F&S and DOC for a 1/2 " bit. Have I gone about it the right way but just used the wrong endmill?
You haven't said if you also adjusted the spindle speed, I'm going to assume you never and that's what allot of people do, they assume slower feed rate equals "safer" but its not always true, especially if they don't understand the feed rate/spindle RPM relationship to chip size/load. Lets do an example on the assumption of Oli not having changed the spindle speed and what those numbers then tell us about the chip size he was producing that may have caused the cutter fail.
To do this we will need to do the maths the other way:
Chip Load = Feed Rate (millimetres per minute) / (RPM x number of flutes)
Feed Rate: 4,000 mm/min
Spindle: 18,000 RPM
Tool Edges: 2
That tells us our chip load is: 0.111 = 4000 / 36000
So we could assume that when the cutter failed for Oli it was because rather than producing proper chips sized at 0.483 it was instead "rubbing" the material away and producing dust relatively speaking, this rubbing then caused the tool to get hot and combined with it just not being up to the job, to then fail.
Oli when you recovered the project using the 6mm solid carbide cutter, what feeds and speeds did you use, the chips in that second video look better, though it dose sound like its screaming a little bit still. The cheap bits are not a total waste of time, you just have to be a little more conservative with them, don't be nervous mate what's the worst that can happen, just "send it" and be confident in your work, we learn from the ways that don't work :-)
Hopefully I've given you enough info to answer your later questions on how to approach F&S etc, if not just ask away that's what the forum is for, for now keep the stepover small just while you find your feet so to speak, once you feel better about it all and get to know your machine and tooling more, then you can start looking to push their limits, I don't think there is an issue with your spindle, I think you would see problems in the bottom of the pocket (finish) if it was out of true etc, Andrew is correct on the using your ears and I'll add eyes (chip size) to help establish if things are running correctly, also another good easy to do tip is to check the cutter after a job to see how hot it is, warm to the touch is ok :)
Key tray looks great, brilliant feeling when you take something off the machine for the first time isn't it :)
Did you get a Jazzy (Dean) machine in the end or something else ?
Re: Endmill failure or wrong feeds and speeds?
Thanks for all the info Lee. I've read it a few times trying to absorb it.
Quote:
You haven't said if you also adjusted the spindle speed, I'm going to assume you never and that's what allot of people do, they assume slower feed rate equals "safer" but its not always true, especially if they don't understand the feed rate/spindle RPM relationship to chip size/load.
Good assumption for the 6mm endmill I used 4000mm/min feed rate 18000RPM and a 3mm DOC, stepover 40%
Quote:
Lets do an example on the assumption of Oli not having changed the spindle speed and what those numbers then tell us about the chip size he was producing that may have caused the cutter fail.
To do this we will need to do the maths the other way:
Chip Load = Feed Rate (millimetres per minute) / (RPM x number of flutes)
Feed Rate: 4,000 mm/min
Spindle: 18,000 RPM
Tool Edges: 2
That tells us our chip load is: 0.111 = 4000 / 36000
So we could assume that when the cutter failed for Oli it was because rather than producing proper chips sized at 0.483 it was instead "rubbing" the material away and producing dust relatively speaking, this rubbing then caused the tool to get hot and combined with it just not being up to the job, to then fail.
Quote:
Oli when you recovered the project using the 6mm solid carbide cutter, what feeds and speeds did you use, the chips in that second video look better, though it dose sound like its screaming a little bit still. The cheap bits are not a total waste of time, you just have to be a little more conservative with them, don't be nervous mate what's the worst that can happen, just "send it" and be confident in your work, we learn from the ways that don't work :-)
With the bit screaming as you suggest which setting would you have adjusted? I'm guessing you would have adjusted the RPM down? I would have probably been tempted to reduce the feed rate. I probably need to practice different settings on a scrap piece of wood to get a better feel for it.
Quote:
Hopefully I've given you enough info to answer your later questions on how to approach F&S etc, if not just ask away that's what the forum is for, for now keep the stepover small just while you find your feet so to speak, once you feel better about it all and get to know your machine and tooling more, then you can start looking to push their limits, I don't think there is an issue with your spindle, I think you would see problems in the bottom of the pocket (finish) if it was out of true etc, Andrew is correct on the using your ears and I'll add eyes (chip size) to help establish if things are running correctly, also another good easy to do tip is to check the cutter after a job to see how hot it is, warm to the touch is ok :)
Lot's of info thanks, The cutter was warm after this project not too hot to touch which is a good sign.
Quote:
Key tray looks great, brilliant feeling when you take something off the machine for the first time isn't it :)
Never get tired of it, it's great seeing a design go from the PC screen as you intended it to.
Quote:
Did you get a Jazzy (Dean) machine in the end or something else ?
Yes mate I did, It's a great machine that Dean and Jared made for me. Really pleased with it.
Re: Endmill failure or wrong feeds and speeds?
Quote:
Originally Posted by
CNCOlly
With the bit screaming as you suggest which setting would you have adjusted? I'm guessing you would have adjusted the RPM down? I would have probably been tempted to reduce the feed rate. I probably need to practice different settings on a scrap piece of wood to get a better feel for it.
Yes mate I did, It's a great machine that Dean and Jared made for me. Really pleased with it.
I'm not sure but the main point is you shouldn't need to guess at any of it, as long as you maintain the known good chip size as you change the feeds and speeds, then everything should to go plan for you, what CAD/CAM software are you using ?
Re: Endmill failure or wrong feeds and speeds?
I used Vectric Aspire for this project.
The penny has just dropped with regard to chip load after your last comment. Chip load and chip size are interchangeable terms. I didn't actually realise that the chip load meant the size of the chip coming off the tool, I don't really know what I thought the chip load value related to. Hopefully, that will help thanks.
Re: Endmill failure or wrong feeds and speeds?
Evening Oli,
Well chip load also known as the Feed Per Tooth is actually supposed to mean the length of material being loaded into each cutting edge, so there can be a difference because you could argue for all the dimensions of a chip: width, length, thickness etc., so chip load is really referring to the length of the chip...
It is to be known as the theoretical length however, as other things like the width of the cut and/or flute edge geometry affect the thickness of a chip. If you measure the thickness of said chip accurately, the thickness you read wont give you the same numbers as the original chip load that was calculated.
Personally I think calling it chip size generalises it and makes it a simpler thing, in the beginning I did the same as you and didnt really give it enough thought so also didnt really know what "chip load" meant, I jumped straight to a basic speeds and feeds chart with no pictures etc, I quickly worked it out from there and since I've always called it chip size to myself and when explaining to people...
We both learnt something from this today, I did underline all of the instances where I called it chip size in my other post, on the assumption that you and others would notice that and get it, however I realise now I should have just made it clearer, sorry about that.
Have you tried cutting MDF yet?, reason I ask is because not many people realise (me included) that if you get the formula right for cutting MDF, it too will produce proper chips, I was really surprised by that and always thought of MDF as a dust only kind of thing to be working with, its quite a good material to learn and "chase" the correct chip on...
Re: Endmill failure or wrong feeds and speeds?
Evening,
All the MDF I've cut so far has just made dust. I've got plenty of offcuts of MDF so probably worth using some of it up to try and get some chips. I think MDF can vary in quality quite a lot? I'd like to give it a go over the next few weeks and might report back with my findings to share my learning experience.
Oli
Re: Endmill failure or wrong feeds and speeds?
Hi Oli,
Yea when you hit that sweet spot with MDF you will definitely know, if you go with any of the "pro" type from any of the top brands you should be good, the cheap stuff from the likes of B'n'Q etc is no good, though they are doing Medite Trade, particularly in the 18mm, again this doesn't machine as good, I would say to anyone go with Medite Premier if you can get it in, otherwise the likes of Build Base and/or Selco do Norbord / Caberwood and this is good enough, again stay off the Trade line with these too.
Ok cool, I'll try and grab some shots of my edge finish for you and maybe a video.
4 Attachment(s)
Re: Endmill failure or wrong feeds and speeds?
Quick update. I got back from holiday midweek and on my return, I received a package containing some new endmills from XCAN - Aliexpress. All excited and stocked up on some lovely new oak boards from the local hardwood supplier I decided to have another go. I snapped the new endmill on my first attempt... I'm clearly driving these things way too hard. Time to take a step back and slow things down. Is there a way to tell if the endmill is actually solid carbide as advertised? Ideally, so I can rule out the chance of it being a low-quality bit. It certainly looks the part. It failed on a plunge almost at the end of cutting two parts out. Unfortunately no video.
Here are my settings, again I thought I was being conservative with the settings 1/2 the chip load that the endmill of this size is supposed to be able to cut hardwood.
Attachment 31373
Some pics of the fail.
Attachment 31371
Attachment 31372
Attachment 31370
Re: Endmill failure or wrong feeds and speeds?
I'd say the plunge feed rate was to much, if your going to plunge with a tool designed for side cutting, its best to ramp into the cut if you can or use a drill operation first to open it up for the cutter to fit inside and then start side cutting. Or you can use a spiral ramp cut, did you use either of those or just plunge straight down into the oak?
Edit:
Is the second pic where the cutter broke in the oak?, it looks like it is and suggests a straight plunge...
