. .
Page 1 of 2 12 LastLast
  1. #1
    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.



    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
    Last edited by Lee Roberts; 09-10-2022 at 11:06 AM. Reason: Added vid

  2. #2
    Some Pics

    Click image for larger version. 

Name:	IMG_20221009_090416241.jpg 
Views:	35 
Size:	178.8 KB 
ID:	31299

    Click image for larger version. 

Name:	IMG_20221009_090134724.jpg 
Views:	34 
Size:	306.9 KB 
ID:	31300

  3. #3
    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

    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
    Last edited by Lee Roberts; 4 Weeks Ago at 09:50 PM.
    .Me

  4. The Following User Says Thank You to Lee Roberts For This Useful Post:


  5. #4
    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...
    Last edited by Lee Roberts; 09-10-2022 at 11:15 AM.
    .Me

  6. #5
    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.

    Click image for larger version. 

Name:	IMG_20221009_103614306.jpg 
Views:	32 
Size:	225.3 KB 
ID:	31302

    Click image for larger version. 

Name:	IMG_20221009_140528010.jpg 
Views:	29 
Size:	356.2 KB 
ID:	31303

  7. #6
    Quote Originally Posted by CNCOlly View Post
    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.



    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

  8. The Following User Says Thank You to the great waldo For This Useful Post:


  9. #7
    Quote Originally Posted by the great waldo View Post
    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.



    Oli
    Last edited by Lee Roberts; 12-10-2022 at 03:09 PM. Reason: Added Vid

  10. #8
    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

  11. #9
    Quote Originally Posted by CNCOlly View Post
    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 View Post
    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 View Post
    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:

    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:

    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
    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 View Post
    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 View Post
    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 ?
    Last edited by Lee Roberts; 12-10-2022 at 10:04 PM. Reason: speeling
    .Me

  12. #10
    Thanks for all the info Lee. I've read it a few times trying to absorb it.



    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%


    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 :-)

    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.


    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.

    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.

    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.

Page 1 of 2 12 LastLast

Thread Information

Users Browsing this Thread

There are currently 1 users browsing this thread. (0 members and 1 guests)

Similar Threads

  1. Help with speeds/feeds please?
    By examorph in forum Tool & Tooling Technology
    Replies: 5
    Last Post: 29-01-2017, 01:54 PM
  2. Speeds and feeds
    By eurikain in forum Workshop & Equipment
    Replies: 3
    Last Post: 26-03-2016, 06:00 PM
  3. Feeds and speeds software
    By suesi34e in forum Swarf & Chip Management
    Replies: 4
    Last Post: 22-03-2016, 10:30 PM
  4. Feeds and speeds
    By dudz in forum Tool & Tooling Technology
    Replies: 0
    Last Post: 26-08-2013, 11:42 AM
  5. Speeds and Feeds
    By Web Goblin in forum Tool & Tooling Technology
    Replies: 0
    Last Post: 20-09-2012, 01:38 PM

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
  •