ok here's the set up. X-2, MACH 3, Gecko 203V, KDN Tools CNC conversion (no backlash, ok I can't measure that low), 2 Flute .500" cutter, 6061 aluminum >.500" plate, Feed 20ipm, depth of cut .020", Aluminum cutting fluid liberaly applied in front of cutting path = SQUEALING

I've sped up and slowed down the cutter speed, increased and decreased the feed rate, it still persist.

Any Ideas???

Also does anyone know of a good speed feed calculator?

How do you figure "Chip Load" per tooth?

Thanks

Smitty

What type of toolholder; generally setscrew type are more rigid than collet. How much tool is sticking out; keep it back to have the minimum length possible.

Chip load per toothis the distance the feed advances during the rotation of one tooth. So if you want a chipload of .005" per tooth on a two flute cutter running at 3000 rpm you multiply .0005" per tooth b y two teeth which equals 0.01" per revolution so at 3000 rpm the feed has to be 30 ipm.

Generally to reduce squealing, actually called chatter, you want to increase the chipload; slower rpm or faster feed. But first make sure your tool is held securely and not sticking out too far.

Incidentally 0.02" depth of cut is a bit skimpy; ten times this should be possible provided you do not run out of hp.

What type of toolholder; generally setscrew type are more rigid than collet. How much tool is sticking out; keep it back to have the minimum length possible.

I have to disagree - for the purposes of roughing and holding the tool still, an endmill holder is more rigid. But for the purpose of chatter, and endmill holder is a wind chime compared to a collet. There's lots of data out there on this.

...But for the purpose of chatter, and endmill holder is a wind chime compared to a collet. There's lots of data out there on this.

Okay give me some links.

There was a recent thread about setscrew type holders that discussed this and I think the concensus was that these are more rigid than the ER, taper collet, type holders. My experience is that collet holders are simply not up to taking the kind of speeds, feeds and chiploads that a setscrew holder can handle.

The correct Collet (LMS) to hold a 3/8 end mill. It is shoved all the way up so that only the cutting edges are sticking out.

So I should be taking deeper cuts? I watch the videos of Hoss doing depth and feed rate test and based my set up on that. He was taking 0.075 at 5ipm and it stalled.

Oh I forgot to mention that the 0.500" plate is held to a second sacrifical plate with some wax paper that I bought for holding parts like this.

I will edit the code to speed the feed rate up some and see if that helps.

Thanks

Smitty

....So I should be taking deeper cuts? I watch the videos of Hoss doing depth and feed rate test and based my set up on that. He was taking 0.075 at 5ipm and it stalled....Smitty

If you have limited power sometimes it is difficult to get enough load to prevent chatter before you stall the machine. And, despite what toastydeath suggests, I think you should try a setscrew holder. If it doesnt't help I will crawl back under my bridge and keep quiet.

I thought only trolls went under bridges, I don't think you qualify as a troll.

I'll have to run down to the corner Tool Shop and get one to try. It's only money at this point, and that's what hobbies are for.

Smitty

When I get a reply that treats me like a troll I will respond as one.:D:D:D

I am not always sweetness and light.

The noise could also come from a dulled cutting edge on the end of the mill or possibly chip welding. I have got a few import endmills that were not all that sharp out of the pack. On 6061 they possibly could have made a squealing sound but they would have been hot also and the surface finish would have been terrible. They were used on large equipment so they were taking heavy cuts and were only used for roughing so it didnt really matter. As far as the Collet vs. Endmill holder debate there is alot of debating back and forth with everyones opinion, to my knowledge there has not been any actual proof in the pudding tests that show one way or the other. This I do know. I have had endmills slightly slide out in a collet during heavy cuts which ruined a few parts in the batch until it was caught. The collet was name brand used very little with the correct size mill and it was tight. The movement was only .0025" but that was enough on that job. For roughing I will always use a setscrew type holder other than that either has proven adequate to me. Alum., Stainless, Toolsteel, Titanium I have used both in each and it is about the same story. With your depth of cut and feed in 6061 I would use either, but if I had a problem I would definately try another holder to rule it out if nothing else comes to light. Just my 2 pennys though.

Okay give me some links.

There was a recent thread about setscrew type holders that discussed this and I think the concensus was that these are more rigid than the ER, taper collet, type holders. My experience is that collet holders are simply not up to taking the kind of speeds, feeds and chiploads that a setscrew holder can handle.

Physics doesn't obey a consensus vote, and just saying an unqualified "rigid" doesn't mean anything in the context of machine tools.

Endmill holders have a higher static rigidity, collet holders have a higher dynamic rigidity. Higher static rigidity means less deflection and overall holding force in the endmill. It won't slip, and it will stay straight at low RPMs. Higher dynamic rigidity means less deflection at high speed, and higher vibration damping at all speeds.

The ASPE has a video series, one of which is Dr. George Tlusty. He determined the equations that describe chatter in machine tools, and it's a very robust presentation on how chatter occurs and why. If you're interested in the subject, I recommend finding the two-part presentation and watching it.

I don't have any webpages on this, nor would I trust any, as the quality of information regarding machine tool dynamics is generally piss poor. The places I've seen quality vibration and chatter analysis of toolholders is in journal articles, personal conversations with people who have a doctorate in the subject, and from people who do high speed machining and have done vibration analysis as part of the toolpath. I believe there was a semi-recent issue of Modern Machine Shop that briefly detailed the advantages of collet holders, but I don't subscribe to it and don't know which issue it was.

Chip load per toothis the distance the feed advances during the rotation of one tooth. So if you want a chipload of .005" per tooth on a two flute cutter running at 3000 rpm you multiply .0005" per tooth b y two teeth which equals 0.01" per revolution so at 3000 rpm the feed has to be 30 ipm.


Howdy Geof,
Typo above, .0005 should be .005 (oops):)

feedrate = rpm x number of teeth x clipload per tooth

rpm = (cutting speed x 3.8) / diameter of tool for mill or workpiece for lathe

Cheers, Jack

Physics doesn't obey a consensus vote, and just saying an unqualified "rigid" doesn't mean anything in the context of machine tools.........etc, etc,

Well I guess I have been put in my place. Okay I will retire to my bridge.

When I get a reply that treats me like a troll I will respond as one.:D:D:D

I am not always sweetness and light.

I like people with lotsa teeth.

Thanks for the replys. I'll play with it when I get to work and see how it goes.

I attempted to use the one in MACH 3.

So any "noise" comming from the cutter is "chatter"? I thought it would be more of a stacato sound for some reason. The finish looked good.

How does depth of cut impact the above calculations? So the Feed Rate and Spindle speed effect chatter, but depth of cut only has to do with hoursepower? I would assume that all three come into play.



Neilw20,

Lotsa teeth, THAT'S WHAT I'M TRYING TO MAKE. Less expensive than a trip to the Dentist, and you can polish 6061 to nice shine. Making my own bling.

Smitty

Neilw20,

Lotsa teeth, THAT'S WHAT I'M TRYING TO MAKE. Less expensive than a trip to the Dentist, and you can polish 6061 to nice shine. Making my own bling.

Smitty


The hard part is welding them in place. Lots of chatter there. ;)

Thanks for the replys. I'll play with it when I get to work and see how it goes.

I attempted to use the one in MACH 3.

So any "noise" comming from the cutter is "chatter"? I thought it would be more of a stacato sound for some reason. The finish looked good.

How does depth of cut impact the above calculations? So the Feed Rate and Spindle speed effect chatter, but depth of cut only has to do with hoursepower? I would assume that all three come into play.



Neilw20,

Lotsa teeth, THAT'S WHAT I'M TRYING TO MAKE. Less expensive than a trip to the Dentist, and you can polish 6061 to nice shine. Making my own bling.

Smitty

I'm going to digitize my false teeth and make some brass ones. (heh,Heh)

....So any "noise" comming from the cutter is "chatter"? I thought it would be more of a stacato sound for some reason. The finish looked good.....

You do mention a stuck pig squealing, that is going to be a high frequency; the tool is vibrating like a tuning fork at a high frequency. But the amplitude of the vibration is going to be very small, so small that its effect on the surface finish is probably not noticeable.

If you calculated the rate at which the tips of the tool are hitting the work piece that frequency is probably in the region you would characterize as staccato; it is this staccato frequency which is exciting a higher harmonic frequency of vibration in the tool.

This is why you play with speed, feed, depth of cut and cutter rigidity. Speed changes the excitation frequency, feed and depth of cut change the amount of deflection which can affect which harmonic is excited, cutter rigidity changes the resonant frequency of the cutter.

Chatter is very complex and it is possible to analyse it mathematically and focus on certain components which can be dealt with separately. If you have a multi-million dollar machine ripping into huge blocks of aluminum for airplane wing spars you spend great amounts of money to maximize chatter-free metal removal so you go into these details. When you are just a little guy like me you work with experience. And when you are feeling generous you pass on advise based on that experience.

Here are a couple more maybe relevant threads:

http://www.cnczone.com/forums/showthread.php?t=49762

http://www.cnczone.com/forums/showthread.php?p=394257#post394257

I agree you probably need to increase the chip load. Unfortunately the X2 is probably not rigid or powerful enough to support a higher chip load on a cutter that size. I don't use endmills over 10mm on my X2 because of this, in my opinion 1/2" is slightly too big for the machine.

Well, the wealth if not the correctness of opionions is always fun.

I noticed that it would be more noticable while the Cutter was moving Left and reduced or completly eliminated moving right. It seemed to happen regardless of Full cutter or just the 75% stepover.

I didn't notice this in my smaller cutters so that could be part of it as well.

I saw the V-8 Block video on YouTube.com Do they cost to much to be called a hobby machine?

So what I gather is I need to get some Aluminum, and test various speeds and Feeds, with different size cutters to find out what the machine can do. Log it all for future, and use those as starter points.

These are HSS Two Flute, Uncoated, from LMS, all of the ones I have are like 3/8 shafts, should I get larger shanks?

OK you know what I have for Cutters, What Should I be Purchasing and from where? I like Made in USA products if that helps.

Smitty

I'm going to digitize my false teeth and make some brass ones. (heh,Heh)

I heard Brass was Gummy to machine. Pun intended.

Smitty

i replaced my gears for metal gears and no problem using a 4 cutter 2.5" facemill. Make sure you have a belt drive or metal gears. My plastic gears lasted all of about 5 mins.

i replaced my gears for metal gears and no problem using a 4 cutter 2.5" facemill. Make sure you have a belt drive or metal gears. My plastic gears lasted all of about 5 mins.

Yup, The first thing I did was get the Belt Drive from LMS.

Smitty

I noticed that it would be more noticable while the Cutter was moving Left and reduced or completly eliminated moving right. It seemed to happen regardless of Full cutter or just the 75% stepover.
Smitty

If you don't know the difference between climb cutting and conventional, you might want to ask some questions for clarification on it...

Without rereading all the posts again, I'd try going with a smaller cutter to reduce chatter and double check how you're holding your work down... If you have a wide flat sheet, you might have to drill a hole in it somewhere to anchor your workpiece in the center...

I build EPS molds on a regular basis and when I have to mill shallow pockets 36 inches long and 5 inches wide by .1875" deep in .500" aluminum plate stock, I always drop a few bolts in and program my tool path around them or else put an ummmmmm.....errrr, nuts, one of those M codes, I can't think, it's not M30, it's the one that is a program stop that waits until you click cycle start again, M02, M01?? Ok, I don't know... (I've taken six months off work starting some new companies and I'm slippin'!!)

Most of the time my chatter results from a combination of speeds and feeds like everyone has said but since you didn't give specs on what you were milling... (Pocket, edge, interpolating a hole, etc.) I think we are all just guessing without knowing the specifics... It wouldn't surprise me in the least if you had a fixturing problem if a smaller tool and adjusting the speeds, feeds and depth of cut don't fix it... (Dull cutter was mentioned by someone too, I'd double check that too!)

It's 2:00 am here and I couldn't sleep, so if I make no sense it's just "chatter!"


Niters~

One more question, you only said that you were using a 1/2" cutter, was it HSS or carbide? Go with a center cutting HSS, which if it's 2 flute, it pretty much has to be center cutting, lol, but anyhow this next suggestion is NOT a rule because I know someone will disagree but typically HSS cuts a little more freely than low end carbide end mills in aluminum... I make custom chopper wheels too for some of the guys on TV and those spokes are EXTREMELY prone to chatter, so I do have quite a bit of experience in eliminating this problem in very unique ways if I could see a picture of what you're cutting...

Assuming cutter rotating clockwise viewd from the top in the normal manner.
You have a 2" Square pocket and are milling around the inside wall.
If you advance forward around the wall in a Counterclockwise direction you are CLIMB MILLING. ie Imagine you had a lot of backlash like on a really old manual milling machine and tried that. As soon as the cutter started cutting it would PULL THE JOB TOWARDS IT, increasing the feed per tooth and possibly break the cutter. Now we have ballscrews wtih vitually no backlash you can cut in this manner. IN METAL it has a number of advantages:
1). A much better finish on the wall of the cut.
2). Less cutter wear.
3). HELPS STOPS CHATTER.

In plastics you usually need to do the opposite!

Some ways to make it work even better:
1). Keep the chips clear with air or compound. Don't let the cutter eat it's own chips
2). Unless the cutter is designed for it, Depth of cut maximum = Cutter Radius.
Using rule 2 you can really push the feed rates to almost rediculous levels if you are game to find the limit.

In summmary
CLIMB MILLING
Each cutting tooth takes a full cut reducing to nothing at 90 degrees of rotation.
NON climb milling
Each cutting tooth takes initially no cut increasing in pressure until the cutter starts to cut. At 90 degrees of rotation cut is at maximum chip thickness.
The INCREASING PRESSURE part of the cut described is where most of your chatter noise is coming from. It RUBS until it cuts. In plastic this rubbing action helps burnish the job and improve the finish, often to a mirror finish.

The bigger and stiffer the cutter the better.
While milling on one side ALL cutters bend away from the job a somewhat.
With small cutters you often have more overhang, so this increases the problem.

Any comments from the gallery?

Yeah, lol, I have a comment and it's, "There is NO WAY I was going to try to explain climb milling verses conventional cutting this late at night!! Thanks for putting that in here and highlighting the specific areas pertaining to this thread!

Here are some photos, of the part and Bit.

2 Flute, HSS, Center Cutting, Non-coated, 3800RPMish, Cutter is moving left to right when it chatters the most, .020 depth at 20ipm

I found the override buttons on Mach 3 so I'll play with that also.

I am using MITEE-GRIP wax stuff to secure the cut piece to a sacrificial piece. The sacrifical piece is clamped at both ends.

I'd actually just like to cut the part out of the center, that would take alot less time. I just havn't figured out enough "CODE" to know how, YET.

Thanks for the assistance with the beginners.

Smitty

I havent used the "MITEE-GRIP wax stuff" so I dont know about that. Directly clamp your workpiece and use the same endmill, slow rpms down to about 900-1200 rpms and depth of cut to .060" at around 10ipm. Try that and if it doesent chatter increase IPM. until you get to having chatter again. You can also change DoC instead of feed. Just a easy way to see if its a workpiece issue vs. tooling. I have a feeling that your piece may be vibrating and contributing to this situation.

I agree, I'm going to bet it's probably a clamping / hold down problem more than tooling at this point... If you could send one more picture from the top view off to the side a little to show how it is attached to the table it would help quite a bit to diagnose this more accurately...

A good rule of thumb is to NEVER use less than three clamping points but my mill has 2000lbs of side thrust and upwards of 3000lbs in Z so it might be overkill for your application but it is a good idea to do anyhow... There are a couple of reasons but one basic one is that three points can be used to describe a plane mathematically and you are trying to mate two flat planes together... The other more important reason is that if there is ANY warp in your part it will take much more of the flex out of your setup resulting in more part to table contact thereby removing much of the resonance Geof talks about in a lot of his threads... Finally it creates a triangular clamping arrangement that is many many many times stronger than clamping at two points which are always in line with one another... (In other words, even if you put one three inches up in Y you still only have two points which by definition create exactly one and only one line...)

HOLY COW!

I totally forgot to mention this because when you do this for a living you never consciencelly think about it, you just assume it and work around it but your stock is just raw stock and it's NEVER going to be perfectly flat unless you grind it which is a pain in aluminum... your particular piece of stock wouldn't be a really ideal candidate to try to mill flat, it theoretically could work but in real life it won't be flat like you think it should be, it'll warp every time unless you're really good AND patient... I hate using absolutes because there are ALWAYS, lmao, exceptions!!

I don't have any experience with this wax you are referring too but I completely agree with maxboostbusa:

"I havent used the "MITEE-GRIP wax stuff" so I dont know about that. Directly clamp your workpiece and use the same endmill"

We can definitely fix this problem you're experiencing, it's not difficult but it takes a little bit of practice and is easy to show in person but harder to explain on a forum...

You'll be up and running soon brotha!!

later~

Ok, last one and I gotta run... Are you leaving .010" for a slower rpm, slower ipm cleanup pass at the end? Even if you're chattering like a three year old on speed you should be able to have an excellent finish if you learn that approach... I sometimes run 150-200ipm at 4500 rpm cutting out forward controls and it howls like a banshee, the advantage is that I save so much time on my cycles it's worth it to me to have one slow pass at the end for cleanup... The parts look scrapped until it does the finish pass... I'm serious, yours look like a million bucks compared to my high speed roughing passes~

I'd still like to see a picture or of your hold downs if possible, I'm not familiar with the layout of the t slots on your particular machine either...

PS
Make SURE you climb cut on your finish pass or you'll most likely get a little rubbing on your finish that looks like #$%^!! Also just for the sake of scale roughly how big was your blank again??

Here is the link to the Wax stuff

www.miteebite.com

I'm using that because the software I'm using won't allow me just to cut the shape and the hole. I'm leaving .01 for a finish pass, 5 IPM

I've attached additional photos and the .TXT file for the part.

Thanks all for the help. This dog will hunt one day.

Smitty

Oh yeah, we can fix these problems! I can't write right now but I wanted to tell you those pictures answered all the questions we need to get you up and running... I'll write more later but the problem is DEFINITELY the setup~

EASY FIXES!!

Thanks for the taking the time to send the pics, I think you'll get a lot better advise from everyone now that we can 'see' the problems...

ps
What rpm's are you running on your finish pass at the 5 ipm??

Alrighty, lets get this thing cutting better:

1.) It looks like your sitting on a piece of 1/8" for your sacrificial stock... You're ok in doing this but the first and biggest problem is that you need to be clamping on the part and not the sacrificial piece underneath... You may need to get your part stock a little oversize from what you currently have in order to accomplish this...

2.) The other possibility is to cut it in two operations if possible... I do not know what your part is supposed to look like finished but it may be possible to machine the hole and the inside area of the right hand side first (green in my picture), then reset up to cut the remaining perimeter... By doing that you most likely could keep your stock the same size you have now or even a little smaller... I'd go smaller after looking at the picture on the left in post #27... You would be better off cutting mostly air than having your cutter fully engaged while cutting...

3.) If you went with #2, which is how I would probably consider doing it in light production, you'd need to make a simple fixture to locate the part both securely and just as importantly accurate... Remember, none of us know your tolerances, surface finish, application, customer or personal standards, etc.

4.) I don't see right away where you could easily cut your shape without a second operation... Don't think of second operations as a bad thing... Much of the time it's much quicker to make double or triple setups to avoid potential problems...

5.) The only thing I would most likely steer clear of for that particular part would be machining the profile first and the inside detail second...



I don't mind taking more time to expound on any of those... I thought it might be a good idea to start here so you can just refer to the number in case of a specific question... I know the descriptions were vague at best but I was only looking to throw out a couple of ideas for everyone's scrutiny!! lol, good luck, you'll be making awesome parts shortly!!

ps
The red is where I'd drill and tap holes in my second operation fixture for my bolts and straps... I make backing plates for choppers EXACTLY like this and it goes super-super fast... It practically takes longer to explain it than to cut them...

Alrighty, lets get this thing cutting better:

1.) It looks like your sitting on a piece of 1/8" for your sacrificial stock... You're ok in doing this but the first and biggest problem is that you need to be clamping on the part and not the sacrificial piece underneath... You may need to get your part stock a little oversize from what you currently have in order to accomplish this......

I figured clamping to the actual part to cut is best. I'm using Alibre to draw it, imprt into MeshCam for the G-Code. I figured I could cut out the entire part and flip it over and cut off around .005 allowing the part to "drop" out. With the thickness of the stock that won't work though. The G-Code cuts all the remaining stock away so I can't just clamp to it.


2.) The other possibility is to cut it in two operations if possible... I do not know what your part is supposed to look like finished but it may be possible to machine the hole and the inside area of the right hand side first (green in my picture), then reset up to cut the remaining perimeter... By doing that you most likely could keep your stock the same size you have now or even a little smaller... I'd go smaller after looking at the picture on the left in post #27... You would be better off cutting mostly air than having your cutter fully engaged while cutting...

So I would disect the G-code and break it up into two sections with a stop feed to move the clamps? Not sure on my discetion skills at this point, that's why I was allowing it to cut all the way around the part as drawn. Please advise.


3.) If you went with #2, which is how I would probably consider doing it in light production, you'd need to make a simple fixture to locate the part both securely and just as importantly accurate... Remember, none of us know your tolerances, surface finish, application, customer or personal standards, etc.

This is for a buddies Kawi 600 to hold his ike stand, pretty loose is what I'm thinking and I love to polish aluminum.:withstupi


4.) I don't see right away where you could easily cut your shape without a second operation... Don't think of second operations as a bad thing... Much of the time it's much quicker to make double or triple setups to avoid potential problems...

In theory I agree, we are hitting a "Skill Set" wall, of course this wall will be reduced in size over the next few years, it's here today. LOL


5.) The only thing I would most likely steer clear of for that particular part would be machining the profile first and the inside detail second...

Makes sense to me, leave the most clamping area of the part avalible and than cut it down. I'm sure after cutting the inner area and the hole, that just mounting it differently would work also.


I don't mind taking more time to expound on any of those... I thought it might be a good idea to start here so you can just refer to the number in case of a specific question... I know the descriptions were vague at best but I was only looking to throw out a couple of ideas for everyone's scrutiny!! lol, good luck, you'll be making awesome parts shortly!!

ps
The red is where I'd drill and tap holes in my second operation fixture for my bolts and straps... I make backing plates for choppers EXACTLY like this and it goes super-super fast... It practically takes longer to explain it than to cut them...

Thanks for the help. I'm sure there are several ways to cut this, part out. I was using software to compensate for lack of knowledge. It looks like I need more of one and less of the other.

Smitty

FYI - this is only the third real piece i've drawn and attempted to cut. That's for future refferance. LOL

**********************************************
2.) The other possibility is to cut it in two operations if possible... I do not know what your part is supposed to look like finished but it may be possible to machine the hole and the inside area of the right hand side first (green in my picture), then reset up to cut the remaining perimeter... By doing that you most likely could keep your stock the same size you have now or even a little smaller... I'd go smaller after looking at the picture on the left in post #27... You would be better off cutting mostly air than having your cutter fully engaged while cutting...


(((So I would disect the G-code and break it up into two sections with a stop feed to move the clamps? Not sure on my discetion skills at this point, that's why I was allowing it to cut all the way around the part as drawn. Please advise.)))
**********************************************




Not really, I wouldn't dissect any code but then again I can import straight dxf into my machine, fill out the conversational programming boxes or have bobcad generate it for me... Lots of options... I'll repost the picture again with more colors and explain what I meant~

I'd clamp her down at the corners and proceed to mill out hole D...

Then I'd program a toolpath starting before B (lead in) and following the green line end beyond C out in space... (lead out)

Now I'd build a little aluminum fixture really quick (if I were going to make these in production) that would have a boss slightly smaller, (0.003") smaller than the diameter of hole D... This will give you two of the three things you need in order to have your part automatically aligned... It gives you a repeatable X and Y coordinate and if you also drill and ream a dowel pin tangent to any point on the green wall inside the hook you'll attain your squareness by rotating your part tight against it... Then you just tighten down bolts into your aluminum fixture at both D and E...

Next program a toolpath starting before A and proceeding along the blue line past B

repeat the procedure again for C to....to....damn it!! Ummm, how about from C following the other blue line out past where I should have put another number, lol... What a dork~

viola, part done!!

However, now that I know you're probably NOT going to do production... You might want to get some more opinions...




AFTER SAYING ALL THAT, here is how I'd build a 'one-off' because the added cost of thicker stock means notta on onesey's



I'd throw a piece of .625" stock in a vice, mill it all but .100" through on ALL the detail, flip it over in the vice and face the backside...

DONE!! LOL~

I would think with some practice you could go from cad file to finished part in well under 45 minutes pretty easily depending on how fast your mill cuts... (I'm estimating mine to take about 3-4 minutes to cut the detail and 90 seconds or less to face the back with an endmill...)

I should have told you to cut it this way first but I didn't think to ask you sooner if it was a one off or production........SORRY!!

I think some of the trouble you are having is with Mechcam. It likes to cut everything. That is actually what it is intended to do. It is just too much cam for simple profile cuts like this. I use Sheetcam for most things I do. It can cut the part out exactly as you have shown in the photo if that is what the finished part needs to look like. However, it appears that you only want the holey fork profile. With a 2D or 2.5D cam package, you could easily mill that profile out of a solid block in maybe 5 to 10 minutes.
There are other free 2D cam packages that you can download and try out.
Meshcam is nice for 3D work, just far too busy for simple profile work.

Leeway,

Thanks I also have Level 2 Dolphin CAD/CAM. but so far have been unable to draw anything meaningful in it to cut. I have Alibre and that makes sense to me. Scary yes, able to make drawings, yes.

I will start digging around for some 2.5D easy to use software also.

Thanks for the advice.

Smitty

I'd try a new/sharp 3 flute cutter, 3/8" and 1/2".
The 3 flutes cut down on harmonic chatter (compared to a 2 flute) without the chip confining problem with a 4 flute during full width cuts.

Whatever, but it seems to me that the squeal problem you are having is primarily due to the cutter you are using.

Pres

Yup, 3 flutes are better for a number of reasons in aluminum, I agree totally but he probably doesn't have the cash to just be blowing on extra EM's until he figures out how to make parts... You can build his part with HSS 2 or 4 flute no problemo...

I'd get a smaller cutter too but let's just get him making good parts first~

I disagree completely on you saying it's primarily the cutter, with a different setup I could cut those with either a 2 or 4 flute without any trouble or chatter... The problem is not being clamped down correctly, look at his pics... I never even had a three flute until last year and I've cut hundreds of hours without too much chatter when I take the time to setup properly...

Yup, 3 flutes are better for a number of reasons in aluminum, I agree totally but he probably doesn't have the cash to just be blowing on extra EM's until he figures out how to make parts... You can build his part with HSS 2 or 4 flute no problemo...

I'd get a smaller cutter too but let's just get him making good parts first~

I disagree completely on you saying it's the cutter, with a different setup I could cut those with either a 2 or 4 flute without any trouble or chatter... The problem is not being clamped down correctly, look at his pics...

If I would have known what to buy before hand I would have picked up the Three Flute types first. Oh well, you don't know what you don't know.

I can throw some cash at the problem, as long as it cures it. LOL

I have the 6 piece set from LMS 1/8", 3/16", 1/4", 5/16", 3/8", 1/2", I picked the 1/2" for rough to get rid of all the material MESHCAM wanted to remove. You have no idea how long it would have taken with a 1/4". Jesus would have returned and it would still be only halfway though.

So for future referance only buy the Three Fluted, HSS, uncoated End Mills?

FYI - that program took 2 1/2 hours to run, ouch.

Still working on how to program the silly thing.

Smitty

I'd go with the coated 3 flute carbides, they are badass!! No comparison in my limited experience with the 3 fluters, you ought to ask others for the best ones, I only have three of them so far...

You don't need them now though, get good first because you're going to break cutters learning all this and HSS is the cheapest way to learn... You don't buy a brand new vette to teach a kid to drive do ya??

Oh crap!! 2 1/2 hours?! Wow!! I don't have any experience on those little mills like yours except a little guy we have that was $20,000 new... I bet yours is similar to that thing only less expensive...

I must be missing something... How in the world does it take that long to cut?? Is it trying to cut everything 3D?? I don't want to spend the time uploading your text file and converting it for my mill so that I can do a visual verification... I wish you didn't live 3,000 miles away, I'd love for you to stop at my shop for an afternoon just to play on the mill to get a feel for setups and such...

Also, why so many lines of code?? It's such a simple part and the geometry is about as basic as you can get... I'm not familiar with your software so I'm of no help to you there but there is waaaaaaay too much code there or that part~ you ought to go to the meshcam forum for help on that aspect of things... Leeway was right...

Man, sorry about adding another post on here but in reality here is how I see it and this is JUST my opinion... If you're a hobby guy not out to run production in aluminum just do yourself a favor and save your money on the endmills for awhile... I said I've had three of those awesome endmills and they were pricey so here is how each one died...

Cutter one had an operator error in an EPS mold, I hit the spindle stop button instead of the drive halt button, they are the same color mounted side by side... Busted!!

The second one died after halting the program and then restarting, I hit go before I hit the coolant on button, (wasn't thinking) and she loaded up a flute and snapped it off almost instantly...

Cutter number three rolled off my desk onto the concrete... #$^$^ #$^^$@ %#$ @#%!!!!!!!!!!!!!!!!!!!!

I bought them on sale but still had over 100 bucks into them... Did they cut nice?? Heck yeah!! Were they better than my old tooling?? Probably to a point, I think they cut faster but only knocked at the most a third off my cycle time compared to a 2 fluter in a perfect world and maybe slower than a four flute by 25%...

One thing they do improve is the chatter and it's obvious just looking at one why it helps... If you picture a two or four flute cutter, the flutes are directly opposed to one another, so if you're fully engaged you are going to be hitting on both sides of the cut simultaneously!! In other words, one side is cutting and one side is rubbing every single revolution on a 2 flute and twice per revolution on a 4 flute, not the most ideal arrangement!!

The thing is that you can normally get around this dilemma with good fixturing and just as important is good chip evacuation with coolant or constant air blast... As mentioned by Pres, the four fluters aren't very good at getting your chips out as 2 or 3 flutes and they load up a lot in the center which is bad bad bad~

I'm tired bro, I gotta get up for Church in the morning and it's after midnight already... My mind is going bye bye, so I hope I made some sense!!

Oh crap!! 2 1/2 hours?! Wow!! I don't have any experience on those little mills like yours except a little guy we have that was $20,000 new... I bet yours is similar to that thing only less expensive...

I must be missing something... How in the world does it take that long to cut?? Is it trying to cut everything 3D?? I don't want to spend the time uploading your text file and converting it for my mill so that I can do a visual verification... I wish you didn't live 3,000 miles away, I'd love for you to stop at my shop for an afternoon just to play on the mill to get a feel for setups and such...

Also, why so many lines of code?? It's such a simple part and the geometry is about as basic as you can get... I'm not familiar with your software so I'm of no help to you there but there is waaaaaaay too much code there or that part~ you ought to go to the meshcam forum for help on that aspect of things... Leeway was right...

2 1/2 hours no lie. I see your Icon looks like a Honda 450, I have a Cannondale, stroked, ported, etc. etc. almost 50hp and when I get her Dyno tuned should break it by a little.

I'll stick to the cheap for learning right now. Yes it is trying to 3D the part out of the center of the stock.

I'm sure some of this could be handled in an Afternoon of Hands on. I'm in SoCal and I'll pay for all the Dr. Pepper you can drink.

I'm playing with Dolphin right now just attempting to get it to only cut the profile out, that brings it down to 25 mins. That's at 20ipm and 0.020 depth with a 1/4" end mill.

Smitty

Here is some reading for both of you:

http://www.mmsonline.com/articles/010101.html

This is along the lines of what toastydeath was referring to, and what I was refrring to when I mentioned big sums of money. It does mention the three flute/two flute difference and AMCjeep is correct in his analogy. There is another application; actually two but they are related, where 3 is better than 2, and that is the number of blades on a wind turbine and the number of blades on a boat/ship propeller, and for the same reason. Although on propellers you sometimes get five blades, but then you don't need to worry about chip clearance. :D

Dude, you're cutting a half inch deep, don't go below 3/8" on your cutter diameter just in case you load up a flute your cutter might survive!! You can easily cut it with 1/4 inch but just to be on the safe side use the bigger cutter, it will only add seconds to your run time~

Yeah it's a 450 but I never bought it, I picked up a limited edition stealth black 800cc Polaris (55hp stock) instead and two months ago bought the limited edition stealth black 700 ranger (40hp stock) 50+ mph top end though with the winch and everything... My shop looks like a SWAT team headquarters!! LMAO, that ranger is fun!! We jump it on my motocross track behind my house, it's 1/2 mile long and 22 feet wide so you can get hauling with two buddies in there and scare the daylights out of everybody!! Just remember to take the water bottles out of the cup holders before lift off, they'll bruise ya!!

That is so funny about the Dr. Pepper, did you read a post I wrote on them or were you just messin' around?! They used to be one of our customers back in the day and I love that stuff!! Have you ever had it in the glass bottles from the Texas bottling plant that still uses cane sugar?? MMM MM MMMMM!!

Good luck~ Keep us posted...

.....We jump it on my motocross track behind my house, it's 1/2 mile long and 22 feet wide so you can get hauling with two buddies in there and scare the daylights out of everybody!!.....

Aw shoot, now I am jealous!!! Half mile...2640', if I am to believe my calculator, we have less than 260 for fooling around on my son-in-laws Kawasaki. But that's enough to scare an old codger like me.:)

Can anyone else get Geofs page to load?? :confused:

I tried it several times and it didn't go...

Don't be too jealous Geof I exaggerated on the length, it's actually 50 feet shorter than I said... LOL, only 2,590 feet until we add the new loop in the spring then who knows!! :stickpoke

Can anyone else get Geofs page to load?? :confused:

I tried it several times and it didn't go...

I just went to my post and it loaded. I also accessed it before doing the post. If you cannot get it to load I have a saved copy which I could upload but that might contravene CNCzone policy.

PM me with an email address and I can send it as an attachment.

That figures, lol, it loads as soon as you posted that, unbelievable... Don't you just love computers?!

That figures, lol, it loads as soon as you posted that, unbelievable... Don't you just love computers?!

Murphy rules!!!!!!!!!!!

That was insanely over my head Geof but interesting enough that I'm going to reread it a few more times with a dictionary, pen and paper next to me though... I understood the basic concepts easy enough but the application of it was a little out of my mental reach tonight (morning, whatever~)

NOW NO more posting until I wake up in the morning, I gotta go to bed!!! Does everyone understand???!!!!!

Geof, that's an awesome link. Thanks for finding it, I didn't know a few of the items in there.

Alrighty folks, I am awake now........carry on!!

:)

Geof, that's an awesome link. Thanks for finding it, I didn't know a few of the items in there.

The Piled Higher and Deeper guy doing that work also mentions that collet holders are preferred over setscrew and he downplays the hydraulic clamping collet holders. My experience, and also the experience of other posters is that setscrew holders are better; I have also looked into the hydraulic holders which allegedly give better tool life because they run truer and vibrate less and have some opinions that they are better than split collet type. In a few weeks I will know because I bought some to use in some heavy hogging of aluminum bars. The ones I have are not hydraulic but elastomeric (very viscous hydrualic fluid you could say). They are made by Schunk so you can go to their website.

I can reconcile the difference between my experience and what Dr Badrawy finds simply because I am working in a different rpm realm. He is above 15,000 rpm and mentions that this seems to be a break point; one of the graphics shows 17,000 rpm as a sweet spot and I thought I had seen 25,000 mentioned but can't seem to find it now (could be a different reference).

I do have one machine that does 15,000 rpm on which we run some parts that are roughed with a 3/4" high helix two flute fully engaged, 0.4" deep running at 10,000 rpm and 120 ipm.; this gives a spindle load of about 90% and makes a lot of noise. I don't really characterize the noise as chatter but there could be a high frequency component that is not audibly detectable. I have taken this cut up to 14,000 rpm and 140 ipm using the overrides but my spindle load goes to 120% and the noise becomes unbearable; think jet airplane taking off.

Unfortunately the roughing with the Schunk holder will probably not be done on this machine because it is fitted with a rotary not vises, so I will only be using 10,000 rpm. I do have a big gantry machine that runs 15,000 rpm but any results on that are not comparable because it is such a different style of construction.

I find this stuff interesting even though I do not really have any direct application. The only reason I am going to be doing this heavy roughing soon is because I need a particular bar profile and have not had time to get a custom extrusion done. It is not likely I will do it again; turning about 60% of the material into chips before starting to make the part is not cost effective.

That was insanely over my head Geof but interesting enough that I'm going to reread it a few more times with a dictionary, pen and paper next to me though... I understood the basic concepts easy enough but the application of it was a little out of my mental reach tonight (morning, whatever~)

NOW NO more posting until I wake up in the morning, I gotta go to bed!!! Does everyone understand???!!!!!

NONSENSE! Anyone who can throw out a word like hermeneutics is fully capable of wading through that stuff.:D

Geof,

Definition of Wading:

1.) to make one's way slowly or laboriously (often fol. by through): to wade through a dull book.

2.) To make one's way arduously: waded through a boring report.

You picked the perfect descriptive word for that one!! Although I wouldn't say it was boring, more like milling~ LOL, bad pun for the day!!

Geof,

Definition of Wading:

1.) to make one's way slowly or laboriously (often fol. by through): to wade through a dull book.

2.) To make one's way arduously: waded through a boring report.

You picked the perfect descriptive word for that one!! Although I wouldn't say it was boring, more like milling~ LOL, bad pun for the day!!

So? You are trying to make a point? You think I do not choose my words carefully?:D:D:D

And any more puns like that will lead me to ostracize you for a period of time.

AMC,

I never joke about four things,

1. Grits - you can't get good ones in SoCal, should be a crime with Milk and Sugar on them.
2. Boiled Peanuts - Can't get any in SoCal, should be a crime as well.
3. Dr. Pepper - I've been drinking it since 1967, Canned only, the plastic bottle change the flavor and you can't get it in Glass bottle, Criminal I think.
4. Jesus Christ - I don't want to Clown god.

Geof - I read though some of that and will have to call my PhD buddies to exlain, lol. I'll be re-reading it as well. Application is different but the basics should hold up.

So let me understand this from my little mill if I buy several of the Tool Holders, I can set each of my cutters into them, this will allow me to set up a TOOL CRIB in Mach 3 or other software for tool paramiters and use that also.

Is there one that people like or works better than others? without breaking into the retirement fund. Are they better for roughing or finishing?

Thanks for everyones time in sharing their experiances to help us beginners.

Smitty

I'm very happy to report that you are wrong about #3!! So hey, call me your NEW BEST FRIEND but you CAN get Dr. Pepper in a glass bottle UPS'd from Texas and it's made from the original recipe with cane sugar like it was originally made way waaaay back... Brotha, you can't get it any better than that!! Just google:

"dr. pepper" texas original

That will probably get you to the website... Hold up, I'll find it, gimme a sec...

http://www.dublindrpepper.com/

There ya go!! Enjoy!!

Just do us all a favor and when you go to mill the tops off the glass bottles, use a three flute cutter so no one has to argue on here about it~

As a sidenote I agree with #4 completely and ironically enough that's half the reason I knew about the glass bottles...

You see, I made all of the bottling valves for the plant in Dublin awhile back and my room mate from Rhema Bible Training Center lived close by to the plant and used to load up on it on his way back to Tulsa from visiting his folks so we had literally an entire refrigerator of Dr. Pepper in the glass bottles nearly constantly!!

AMC, for the link to the original Dr. Pepper drink. Ahhh, Dr. Pepper, quads, and God, does it get any better than that, nope.

I wonder if they give you a price break for a pallet?

Back to the question.

Seems that best way to determine the parameters of the machine with Paticular cuttes are Buy some Large Scrap pieces. Write some code to keep constant RPM, Depth, % of cutter engagement, Direction of cut, Feed Rate. Than test the ONE of the above while keeping the rest constant. Run until Chatter happens and document everything. Keep for future referance.

Being that this is a little bitty sucker the MAX RPM is around 4,500 run it topped out first and come down 500 RPM per test?

Sound right?

I'll assume to stay away from the 3 Flute End Mills on E-Bay, right?

Smitty

I can't answer that about Ebay, there a lot of guys here with more experience than me about which ones to buy~

....Seems that best way to determine the parameters of the machine with Paticular cuttes are Buy some Large Scrap pieces. Write some code to keep constant RPM, Depth, % of cutter engagement, Direction of cut, Feed Rate. Than test the ONE of the above while keeping the rest constant. Run until Chatter happens and document everything. Keep for future referance....Smitty

Better be careful here; you are starting to get all logical and scientific. That is supposed to be reserved for us guys with all the initials after our name. :D

Better be careful here; you are starting to get all logical and scientific. That is supposed to be reserved for us guys with all the initials after our name. :D

Geof,

I have four letters after mine.......... NOOB

I have to make a trip though our machine shop, Not as helpful as I'd like them to be, but they are on the clock. They have large pieces of 1" thick Aluminum and Mag laying around that I have been liberating. I'll grab some of them and start testing.

I'm sure that after I run some test piecies I'll have a better idea of what the machine can take. I think Hoss actually has some of the programs written, so I'll ask if I can borrow them.

Thanks for all your help. The link you provided was quite interesting. I'm a Fiber Optic Guy, but we do have dynamic shakers, we use them to test all sorts of items. 400 Gallons of water in a Rocket Fuel Tank get the Earth moving. I'll see if one of thier portable set ups can read the fequencys that were mentioned in the article.

Smitty

As far as ebay cutters go, the ones sold by 800watt are okay. I use them to do basic milling stuff of aluminum and softer steels. They are fine if you are going to side mill or pocket or even an occasional slot cutting. The only time I have any problems with them is when I dont use coolant or am cutting hard steels. Heres a pic of one after trying to face my lathe tool holder. For what you pay, I think mine cost 10 bucks for ten, they work great for nonprecision work and as throwaway cutters.

If you want to try 3 flute cutters I was just looking through my J&L Industrial catalog and they have 3 flute HSS from $15 and Carbide from about $35. They are name brands like Kennametal and Niagara. They also have alum. specific high helix bits in 3 flute. Example Kennametal 3 flute 30 degree helix centercutting single end 3/8" coated carbide $27.13. 3 flute Hertel HSS centercutting single end 3/8" uncoated $15.44.

I did buy some 1/8" 3 flute cutters from 800Watt on Ebay. As mentioned, they are great for light easy machining. Also good when learning your feeds and speeds. These were a little over $1 each when including shipping. I still have about half of these little guys left. I snapped the others with too high of feeds. Just 1/8" though. I have snapped high dollar 1/8" end mills too for the same reason.

I liked these so much I ordered some in 3/16" as well. I still have some higher quality US made end mills, but won't use those until all my Gcodes are fine tuned.
This little video is using one of these 1/8" 3 flutes from 800Watt. My camera no longer records sound for some reason, so I have to add music. ;)

http://www.youtube.com/watch?v=7jRaXnqlxKQ

My Fog Buster unit should be here in a few minutes. That will take me a little while to get it set up. I have included a PDF of the silly little part I'm attempting to make.

This is like my Golf Game, 119 bad shots and the one good shot will keep me playing.

AMC,

Thanks for the link to Dr. Pepper, I ordered two cases of the GLASS Bottles. Wife just called and asked what the $81.00 was for. LOL

Smitty

Whoa!! That is the highest scrap rate on record I'd venture to guess!!

Good luck with that :eek:

We'll have to get Geof to use his big ole' calculator to give us the exact percentage but less than 1% is pretty stinkin' low!! I shoot for at least 6.4% good parts or I sub it out :)


HOLY CRAP $81 for pop in a bottle, roflmao... Dude, who you trying to kid, you can afford any cutters you want!! (chair):wave::rolleyes:

AMC,

The Dr. Pepper arrived by UPS today, 2 cases, is that enough to brib you into stopping by California? It should be cold in an hour.

I figured out some of the issues, I am attempting to redo the tool path using Dolphin and some go around commands.

Well see, how it goes. I have enough material to start testing cut depth and speed now, so maybe this weekend I can run the programs Hoss e-mailed me and post those results.

I ordered some three Flute cutters from 800watts to play with. They should be here in a week and than I'll rerun the speed test.

Smitty

If you are interested in getting some good 3 flute mills J&L Industrial that I quoted prices on earlier has a 35% off sale going on just on end mills.

AMC,

The Dr. Pepper arrived by UPS today, 2 cases, is that enough to brib you into stopping by California? It should be cold in an hour.

I figured out some of the issues, I am attempting to redo the tool path using Dolphin and some go around commands.

Well see, how it goes. I have enough material to start testing cut depth and speed now, so maybe this weekend I can run the programs Hoss e-mailed me and post those results.

I ordered some three Flute cutters from 800watts to play with. They should be here in a week and than I'll rerun the speed test.

Smitty

Since you're a Dr. Pepper fanatic, what did you think?? Did you like it from the original recipe?? What about finally being able to drink it out of a glass bottle again?? It's not that I'm not interested about your mill, lol, I'm just curious how it was after droppin' that kind of cash on some soda, lololol... That's crazy!! :banana:

I got to thinking about your offer and was on priceline getting ready to confirm my airline tickets when this little voice in my head says, "Carl, if this guy was willing to drop $81 on soda, he might be crazy!!" So thanks for the offer but I guess I'll hold off until the real Doctor Pepper can send me your psychiatric evaluation~ :stickpoke

:)

Let us know how your test cuts go this weekend... Oh, who's Hoss?? Did you get on the other forum to get help with programming??

Good luck!!

Hoss is a member on here. He has designed up CNC plans for the X2's and ATC and alot of other items. He seems to be real knowledgable on the unit. He has helped me and others out countless times check out his site. www.hossmachine.com.

Since you're a Dr. Pepper fanatic, what did you think?? Did you like it from the original recipe?? What about finally being able to drink it out of a glass bottle again?? It's not that I'm not interested about your mill, lol, I'm just curious how it was after droppin' that kind of cash on some soda, lololol... That's crazy!! :banana:

I got to thinking about your offer and was on priceline getting ready to confirm my airline tickets when this little voice in my head says, "Carl, if this guy was willing to drop $81 on soda, he might be crazy!!" So thanks for the offer but I guess I'll hold off until the real Doctor Pepper can send me your psychiatric evaluation~ :stickpoke

:)

Let us know how your test cuts go this weekend... Oh, who's Hoss?? Did you get on the other forum to get help with programming??

Good luck!!

Original is not as sweet as the cans I drink now. Glass is the only way to go though it doesn't get warm as quickly although I drink it to fast for that to happen anyway. $81 for the Dr. Pepper only once in a great while.

If you ask the wife about my mental stability, depending on the day it could go either way. It would be nice to have a small local machine shop to watch and ask question of. Mentorship would be nice and would probably save me some money as well.

I was informed that my Brother in Laws 25 wedding anniversary is this weekend so maybe after church I can knock them out. It would be interesting to have several people do it on thier X-2 to see the performance of the various configurations.

I believe Hoss thread is X-2 finished for now maybe, it has the highest post and read count in this section.

Smitty

Just out curiosity, how much does a guy have to dole out (ballpark with delivery/tax/etc.) minus tooling since I have all of that?? Where do I go to get all the specs on them??

I'm asking because I have a 'pro light' but it's the only mini mill I've ever used... lol, I can't remember if said this before but at the risk of being redundant, my little mill weighs about a third as much as the coolant in my regular mill!! Are you liking the product thus far?? (Not counting software and setup issues, I just mean the quality of the mill itself...)

I'm dropping the pro light off at a friends sign shop for awhile to teach him the basics of 3D machining and programming... My mini uses standard R8 collets, what does yours use?? The same, ER style or proprietary holders?? Can you get rotary fourth axis on it?? Oh, is the spindle programmable??

Sorry for all the questions but they might have 2 more buyers up in Kalamazoo if it seems like a good unit, although that little Tormach looks kind of interesting to me too...

So is the newer sweeter Dr. P more to your liking or do you like the cane sugar just as well?? We have stewarts and jones soda in Michigan and they're both better than anything else I've ever had... They probably make 30 different flavors between the two companies... (Saves on shipping since the store is 4 doors down from my shop, lol, I just jump in the S.W.A.T. ranger and go grab me some... I can't even hit 50mph on the way there or I skid past it every time, lol~)