# Spindle speed



## Geerbangr (Dec 28, 2017)

Hey guys!! I have a small job to do on aluminum and I’m wondering about spindle speed. Spindle speed=3.82xsfm/diameter. 

So that equates to 1528 rpm using a 1” bit. Here’s the problem, my closet spindle speed is 1100 or 1900. 

So with that being said can I cheat the system here and use the lower spindle speed of 1100rpm and slow the sfm down? 

I don’t want to use the 1900rpm speed because that’ll burn the bit up, correct?


----------



## Downunder Bob (Dec 28, 2017)

G'day, you don't say if you are using cutting fluid / coolant. If you're cutting dry I'd slow it down, if using flood coolant you could try the higher speed and see how it goes. I assume you're plunge cutting in one step, probably safer to slow it down you'll get more torque, you don't say what machine, HP etc. When the theoretical ideal speed is in the middle like that it is usually better to try the slow one first, Theoretical speeds are just that theoretical, it's a bit like the speed limit on the road that's the maximum, but you don't have to go that fast. What would you do if it was only 1/2" the theoretical speed would be twice what the lathe will do, so what do you do now, just go with what you have.
Downunder Bob.


----------



## Geerbangr (Dec 28, 2017)

Hey Bob thanks for the reply. I just have a cheap 20” enco benchtop mill. As far as cutting fluid what would work the best with aluminum? Wd40 or something like that? 

I have a 2” wide 2” deep 4” long cut I need to make in a 4” piece of aluminum round stock. I can make several passes so it’s not like I’m trying to cut the max cut all at once. 

Is silicone spray good for lube when milling?


----------



## Downunder Bob (Dec 28, 2017)

Geerbangr said:


> Hey Bob thanks for the reply. I just have a cheap 20” enco benchtop mill. As far as cutting fluid what would work the best with aluminum? Wd40 or something like that?
> 
> I have a 2” wide 2” deep 4” long cut I need to make in a 4” piece of aluminum round stock. I can make several passes so it’s not like I’m trying to cut the max cut all at once.
> 
> Is silicone spray good for lube when milling?



G'day again, I'm not familiar with your machine, and I haven't done any milling for years as I don't haver access to a mill, Plaanning on building a mill attachment for my lathe. 

Also on machining Alumimium it's something I rarely do, mostly steel. But I've heard WD40 is good, Kerosine also. Standard approach when in unfamiliar territory start low and slow, and let your machine tell you what it is happy doing. 

Your 1100 rpm is good place to start Is your cutter HSS or carbide? Carbide needs to run really fast 4-5 times that of HSS, and requires much more HP / torque. If the cutter is bogging diown halve the speed and try again. 

Remember Half the speed gves you twice the torque. keep the feed and depth of cut low and gradularly increase one or the other. If your machine is small, and as you say cheap, you'll probably run out of torque and rigididty before the cuts get too big, but listen to the machine. Let it tell you what it can and can't do, that way you'll learn more about your machine. If the machine is complaining, back off.


----------



## Jake2465 (Dec 28, 2017)

I mess with aluminum almost exclusively. I have seen that doing exterior contouring with a conservative width of cut does not seem to be too problematic, but doing internal pockets that would require a high percentage width of cut is where you could run into trouble. By nature, those cuts seem to produce a lot of heat. without some kind of cooling, I would tone down the rpm and run a feed that would be in the neighborhood of 0.001" chip load. 

Working with aluminum is basically a heat game. Milling can easily produce local area heat beyond the melting point of aluminum. In a way it is kind of funny because aluminum is easier to machine than steels but at the same time harder because of the heat constraints. Also, doing deep pockets can pose problems with chip recut which makes it worse. 

If you have a piece of spare aluminum that you can sacrifice, then I would try this: give the surface a spray of water or WD-40 (heavy coating is not required) and try out your operation. Have the spray bottle handy and with each subsequent pass, give it another little spray. Also, aluminum hates high RPM and low feed rates. If you start rubbing the tool more than cutting, then the aluminum will turn into jelly and claim your end mills life .

I like to use this online calculator for my chip loads:

http://www.monstertool.com/monster_tool_calculators.html

Hope this helps. Good luck!


----------



## mikey (Dec 28, 2017)

G, as a general rule of thumb, use the next lowest speed below your calculated speed. BUT as in most things machining, it isn't that simple because your calculated speed depends on many factors and since efficacy and end mill life are greatly dependent upon the correct speed, your calculations are important.

What you are calling a "small job" is a 2" wide X 2" deep X 4" long cut in aluminum - to me, that is a big cut. You indicate that you are using a 1" OD end mill in a benchtop milling machine. That is a big cutter being used in a machine that is somewhat limited in rigidity and power. Most cutting guidelines and calculators do not take the mill into account; they assume you have all the power and rigidity needed to make the cut so if this is not your reality then you need to make adjustments and slow down.

I assume you are going to plunge cut the center and then widen the slot to size. If so, then you are making an initial slotting cut and then two profiling cuts. Slotting and profiling cuts have different cutting speeds. For slotting cuts, it depends on your axial depth of cut. For profiling cuts it depends on both your axial and radial depth of cut. Granted, this fine differentiation may not matter much when all you have to adjust speed is a pulley system but on a variable speed mill, it does make a difference.

Add to your depth of cut, your feed. If you have a DRO and power feed then you can calculate your feed in IPM. If you do not have a DRO and/or are cranking manually then you will need to do it as Bob indicated above - feed by hand and feel for a slight resistance to the feed.

Since your question is about speeds and not about how to use an end mill, I am attaching some guides from Niagara Cutters that will be useful. It addresses the speeds used for various radial and axial depths of cut for different materials. Have a look.

The other thing I wanted to add is that for this kind of job, a roughing end mill is more useful for hogging. Your finishing end mills will last much, much longer if you use roughing end mills to debulk the stock first. I would use a coarse pitch rougher for this job and also use a stream of compressed air to clear the chips and cool the cut. Oil/WD-40 is okay but it tends to clump the chips and makes it harder to clear them so I prefer air for slotting cuts in aluminum. Note that speeds also vary for both roughing and finishing end mills.

Good luck!


----------



## Geerbangr (Dec 29, 2017)

Thanks for the replies fellas. I have not yet purchased the cutter I’ll use to do the job. I’m sure you guys can tell I’m pretty green at machining. I do have a dro and I do have auto feed that I will install for the x axis. So with those file links Mikey that should help with the process. 

My plan is to use a roughing bit to hog out the heavy stuff then complete the job with a finishing bit.


----------



## Aukai (Dec 29, 2017)

Just on a side note, are you a YB member?


----------



## Geerbangr (Dec 29, 2017)

That’s me!!


----------



## Aukai (Dec 29, 2017)

Don't tell them your here then    LOL


----------



## Geerbangr (Dec 29, 2017)

I’m fairly certain that kind of behavior would be frowned upon here.


----------



## Aukai (Dec 29, 2017)

Ya think


----------



## Geerbangr (Dec 29, 2017)

Here’s my little handy dandy mill. I have a power feed I’m going to install next time I’m home on leave.


----------



## mikey (Dec 29, 2017)

Aukai said:


> Just on a side note, are you a YB member?



Curious - what is YB?


----------



## Geerbangr (Dec 29, 2017)

A car website.


----------



## mikey (Dec 29, 2017)

So why would you not want it known on the YB forum that you're a member of HM? I know I'm missing the reference.



Aukai said:


> Don't tell them your here then    LOL


----------



## Geerbangr (Dec 29, 2017)

I think Aukai’s point is HM doesn’t need those yahoo’s here. It’s all good.


----------



## mikey (Dec 29, 2017)

Oh, okay. I'm sorta' dense so you have to forgive me.


----------



## Aukai (Dec 29, 2017)

LOL some of them can be hooligans, and keyboard commandos. This way the mods do not have to officiate. There are some very knowledgeable automotive types there, but minimal behavior guidelines.


----------



## Alan H. (Dec 29, 2017)

Aukai, you speak the truth.  I looked earlier and it was entertaining but not my cup of tea.  Not that I was offended but I just prefer to get to the kernels of knowledge a bit quicker and not have to filter too much turbidity out of the water first.


----------



## 4GSR (Dec 30, 2017)

We don't care if your a member on other forums.  But your on the best forum out there!


----------



## ddickey (Dec 30, 2017)

Nice links Mikey thanks. A little confusing as I'll have to study those. Axial depth radial depth /2,3,8 etc.


----------



## mikey (Dec 30, 2017)

Geerbangr said:


> Thanks for the replies fellas. I have not yet purchased the cutter I’ll use to do the job. I’m sure you guys can tell I’m pretty green at machining. I do have a dro and I do have auto feed that I will install for the x axis. So with those file links Mikey that should help with the process.
> 
> My plan is to use a roughing bit to hog out the heavy stuff then complete the job with a finishing bit.



2" deep means a long end mill, and a long end mill is going to deflect. If the sides of the slot must be accurate then consider a carbide end mill; it will deflect less. Carbide is not mandatory but if you opt for HSS then lighten your cuts accordingly. The flute length must be long enough to span the depth of the cut and it would be wise to use an end mill diameter that will handle that length; I should think that a minimum diameter would be 3/8", no less. Ideally, you want to use a High Helix end mill to pull chips out of the cut.

If this is to be a through slot and you can accept radiused corners then I would drill holes at all four corners and saw out as much of the slot as you can. Then use a rougher to bring it close to size, maybe 0.050" of material to finish up. This gives you enough meat to remove the serrated marks left by a roughing end mill. Then take light finishing passes to bring the slot to final size. You may be able to get away without the rougher but 2" is a deep cut, deep enough that deflection is a real concern so I would personally use the finisher to finish only.

If the cut is a pocket then you have no choice but to hog it out with end mills. I would use a rougher to debulk the pocket and finish with high helix end mills. 

I wanted to remind you that long end mills deflect less when held solidly in an accurate collet. Not many hobby guys can afford shrink fit tooling so an ER collet is the most affordable option. If you don't have an ER chuck for your mill then I suggest you consider one, along with high quality collets.

You can do this. Just take your time, think things through, buy the right tooling and you'll do fine.


----------



## Geerbangr (Dec 31, 2017)

Mikey, I’ve chose to use a 3/4” cutter because I can get closer to the correct bit speed with my machine. I’ve been contemplating using a saw like you mentioned for cropping out the bulk of the material so I don’t have to wear my bits out. 

I only have hss bits so I’ll use a roughing bit to remove any bulk, then finish the cut with the finishing bit. 

Once again thanks a million for sharing your wealth of knowledge.


----------



## Geerbangr (Dec 31, 2017)

Mikey I did not see the last part of your post on ER collets until I posted above. Care to educate me on what a ER collet is/does? 

I’m going to go out on a limb and say extended reach is what the ER represents?


----------



## 2volts (Dec 31, 2017)

The "ER" collet system, developed and patented by Rego-Fix in 1973, is the most widely used clamping system in the world[3] and today available from many companies worldwide. The standard sizes are: ER-8, ER-11, ER-16, ER-20, ER-25, ER-32, ER-40, and ER-50. "ER" came from an existing "E" collet which Rego-Fix modified and appended "R" for "Rego-Fix". The number is the cavity opening diameter in millimetres. ER collets contract over a range of 1mm and are available in 1mm or 0.5mm steps, so a range of ER collets can hold any cylindrical shank, metric or imperial. ER collets may also be used on a lathe to hold work pieces.[4]

From Wikipedia.


----------



## Downunder Bob (Dec 31, 2017)

Geerbangr, what were you planning to hold your cutter in? Hoping you weren't planning to use a drill chuck, Please don't even think about . it. 
A drill chuck is not rigid enough, they tend not to run very true, nor do they have sufficient clamping force to hold a milling cutter, the cutter wil most likely walk out and ruin your work piece, probably break your cutter and damage the chuck, and maybe damage your mill.

The ER collet system is the best one to use. Assuming your mill spindle has a morse taper, what size us it? If not an MT what does it have? And what size is the spindle bore hole for the draw bolt? Always best to use the largest that will fit.


----------



## mikey (Dec 31, 2017)

Geerbangr said:


> Care to educate me on what a ER collet is/does?



The ER system is the most commonly used method of holding an end mill in a milling spindle. It uses a chuck with a special nut at the front that compresses a slotted ER collet circumferentially to rigidly hold the shank of a milling cutter. A good collet will hold an end mill quite accurately, with run out within 0.0001" or less. While it is not the most accurate way of holding tooling, it is the most effective way that is within financial reach of most hobby guys. A search on HM will turn up gobs of discussions about ER chucks and collets. 

I raised the suggestion because of the longish cutters you will need to use. All end mills deflect all by themselves, especially longer ones, but you can minimize it by holding it solidly and accurately; an ER chuck is the most effective way to do that in light of cost. End mill accuracy and tool life will be enhanced, and this holds true for any cutter you use so it is a wise investment when tooling up your mill. 

I suggest you educate yourself about these chucks and collets. I assume your mill has an R8 spindle bore and chucks are readily available to fit it. It is a simple matter of choosing one and then choosing decent collets to fit it. If I were to buy one today, I would be looking for an ETM or Glacern ER-32 chuck. Why ER-32 and not a smaller or larger size? Because it will allow you to use cutters of a size that your mill can handle. An ER-40 will go larger (up to 1" shanks) but that would really push the rigidity limits of your mill. The collets you choose greatly affect accuracy so research this before purchasing. I would suggest Techniks collets as a reasonable option.

I should mention one tooling system that you might consider - the TTS system from Tormach. This is Chinese stuff and not of the quality of makers like ETM, Rego-Fix or Glacern. The big advantage is that it allows you to use different tooling options that are reasonable in cost. Their ER-32 chuck is less than $40.00 and is more than accurate enough for most hobby guys when good collets are used. There are many adapters for tools that fit their system so its worth a look.


----------



## Geerbangr (Jan 1, 2018)

Thanks fellas for replying. My mill uses R8 collets currently. I would not use a drill chick to hold the cutter. So what you guys are saying is the standard R8 collet isn’t really sufficient enough for my mill and I should step up to the ER cutter? Or is the ER collets just needed for long reach applications?


----------



## Geerbangr (Jan 1, 2018)

Oh and Happy New Year fellas!!


----------



## mikey (Jan 1, 2018)

Geerbangr said:


> Thanks fellas for replying. My mill uses R8 collets currently. I would not use a drill chick to hold the cutter. So what you guys are saying is the standard R8 collet isn’t really sufficient enough for my mill and I should step up to the ER cutter? Or is the ER collets just needed for long reach applications?



The key reason I suggested an ER system for your application is because ER chuck/collets dampen vibration better than most other available systems. When using longish cutters, this matters. They also dampen shorter end mills and other tooling so its a good system. The collets are available in increments of 1/32" so just about any tool you are likely to use can be held accurately. These collets can compress down about 0.040" and still hold solidly, albeit with a bit less accuracy so small variations in tool shank size won't bother an ER collet.

Consider also that a high quality collet, like a standard model Rego-Fix, has a run out of 10 microns or less. Their precision collets have 3 microns of run out. I don't know what an R8 collet runs out at but I'm pretty sure it isn't in a comparable range. 

There are many reasons why ER collets/chucks are the commonest tool holding system in the world - fast and easy to use for a wide range of tooling, accurate, damps vibration well, and is probably the most accurate chucking system design out there. You can get collets in both Imperial and Metric sizes so just about any cutting tool you are likely to use can be held securely and accurately. 

Is the ER system perfect? No, it's not. If you're doing a lot of heavy cuts that generate a lot of vibration then it isn't the best choice; heat shrink holders would be better. However, for almost any work that a hobby guy is likely to do it is a very good option. 

You can use an R8 collet. It won't hold an end mill as securely as an ER collet, will not be as accurate, will not damp as well so accuracy and tool life will be reduced. For a hobby guy making a cut in aluminum, an R8 collet may be just fine so I am not saying you should not or cannot use it; I am saying that if I were using an end mill with a 2"+ flute length and needed it to cut accurately, I would use an ER collet to hold it.


----------



## Geerbangr (Jan 1, 2018)

I’ll pick up a ER collet system Mikey. You’ve more than explained why it’s a better system than the typical R8 collets. I went to Tormach website and found a 6 collet pack but no chuck for R8 spindle. I’ll have to call them Tuesday for they are out for the holiday.


----------



## mikey (Jan 1, 2018)

Geerbangr said:


> I’ll pick up a ER collet system Mikey. You’ve more than explained why it’s a better system than the typical R8 collets. I went to Tormach website and found a 6 collet pack but no chuck for R8 spindle. I’ll have to call them Tuesday for they are out for the holiday.



Let me back you up a little here to explain the TTS system. It uses a 3/4" R8 collet with the nose flattened. This allows all their tool holders, which have 3/4" shanks, to fit into this special collet and are drawn up solidly and repeatably in it. You can buy adapters for drill chucks, boring heads, fly cutters and so on. They also have end mill holders and ER chucks that fit into that 3/4" collet. The key attraction of the system is repeatability and speed. To change tools, you simply loosen the drawbar and pull out the tool, then insert the next tool and tighten the drawbar. You do not need to change collets or bang things loose. In addition, when the tooling is set to a specific projection or stick out, it will maintain that projection from the tool holder when you switch tool holders. Very nice system. Their tools and adapters are Chinese, with Chinese levels of accuracy, but they are actually pretty good. Just as important, they cost what Chinese tooling usually costs and that is a big plus.

Now, with that said, there are better ER chucks out there that have an integral R8 shank. My most accurate ER chuck is an ETM chuck from Israel. When used with high quality collets it is nearly as accurate as my spindle is. My spindle has less than 0.0001" of run out and a ground pin held in this chuck/collet system will hold that ten thousandths run out. So, the chuck and collet are accurate but so is the ETM collet nut.

You will discover that accuracy with these collets depends on good quality collets and good collet nuts, all else being equal. Makers of good nuts are Rego-Fix, ETM and Techniks. There are also ball bearing nuts but I don't have experience with good one; just the Chinese kind and I am not that impressed with them.

One chuck that I want to try someday is the Glacern line of ER chucks. Their advertised accuracy is very good and the guys here on HM that have them seem to be very favorably impressed. If I'm not mistaken, Glacern has the rough castings done abroad but does the final machining here, in the US. Their cost is very competitive and I've been meaning to buy one just to find out for myself. 

So, my suggestion is to NOT rush into this decision. You might want to ask the HM membership about which ER chuck they recommend and why. Collets are just as important, as are the nuts used on the chuck. I have my opinions on all of this but it is important to hear from the guys.

Just one more thing. ER collets are often used on the lathe for work holding and do an adequate job of it. However, run out on the lathe is not nearly as critical and you can get away with an import collet set. On the mill, accuracy counts and there I recommend you suck it up and buy a decent set of collets. It will cost you but you will recover the cost over time because your tooling will be more accurate and will last longer. 

Do more homework, talk to the guys and then decide on what to buy. You will often find some awesome deals on ebay and that is where I would search first.


----------



## Geerbangr (Jan 1, 2018)

Ok I’m getting a little confused now. If I buy a R8 ER32 chuck and a set of collets from 1/16”-3/4” I could use my existing different size cutting bits, correct?

Or are you suggesting a R8 ER32 chuck that only accepts 3/4” shanks?


----------



## Aukai (Jan 1, 2018)

Happy new year too....


----------



## Boswell (Jan 1, 2018)

My understanding is that the R8 defines the interface between the tool holder and the machine. Specifically a Taper and possibly a keyway location. the ER refers to the way the tool holder holds the actual tool.  So for instance I have a PM45M-CNC mill that accepts R8 tool holders. I have a number of R8 ER-16 tool holders and the appropriate ER-16 collets for the various diameter cutters that I have. 

Happy New Year


----------



## Boswell (Jan 1, 2018)

Geerbangr said:


> Ok I’m getting a little confused now. If I buy a R8 ER32 chuck and a set of collets from 1/16”-3/4” I could use my existing different size cutting bits, correct?
> 
> Or are you suggesting a R8 ER32 chuck that only accepts 3/4” shanks?




You are correct in that you can use one R8 ER32 tool holder and then the collets to swap out for the different tools you have. You must have the exact size of collet to match the cutting tool.  If you find that you are using a specific cutting tool more often that others then you can purchase another R8 ER32 and the specific collet you need to hold that tool, then you can leave the cutter in the R8 ER32 all the time, making tool changes faster. I have about a dozen dedicated R8 ER32 holders dedicated to specific tools.


----------



## mksj (Jan 1, 2018)

There is a range of clamping with ER collets, so it is often suggested to purchase a 1mm increment set, to cover both imperial and metric end mills. But in my experience, the accuracy suffers, so I recommend purchasing collets sized to the specific size shaft you want clamped. I use two ER sizes, an ER-40 1/32 set that serves as a holding system on my lathe, and on my mill an ER-32 1/16" set along with a few dedicated metric sizes that I commonly use. On the mill, most end mill shanks are standard sizes, so you probably would do just fine with a 1/8" increment set. One negative aspect of the ER system is the size of the holder/nut should you need to mill deep in a pocket. If going to dedicated end mill holders, then a R8 end mill holder system would be less expensive and have a narrower holder. Something like a Taiwanese Sowa end mill holder would be around $40 each. Some feel that the end mill holders may have slightly higher TIR then say an ER system, but insignificant at our level of work.

As Mikey outlined, ETM/Iscar, Rego-Fix, Lyndex if you can find them at a reasonable price are high quality. Some of these show up at auctions as sets, lightly used at a fraction of their normal selling price, so worth considering. I would also recommend Shar's (precision nickle plated), Galcern, Sowa, Tecknics, Bison as new mid level priced alternatives that are very well made. My ER-32 R8 chuck is Glacern, ER-40 R8 and MT3 Shar's both have almost undetectable runout. A high quality nut does make an measurable difference in both the TIR and tightening the nut to the proper torque.  On ER collets, it does pay to get better quality collets, at least for the sizes you use frequently.  If I were to recommend a mid priced ER set, I would go with the Tecknics high precision set. There is a significant difference in both the clamping characteristics and TIR between the inexpensive collets and higher quality versions. This has been stated repeatedly, but you must always snap the ER collet into the nut first then thread it partially onto the ER chuck, then insert you end mill and tighten. Failure to snap the collet into the retaining ring will result in collet misalignment/clamping.


----------



## mikey (Jan 1, 2018)

Geerbangr said:


> Ok I’m getting a little confused now. If I buy a R8 ER32 chuck and a set of collets from 1/16”-3/4” I could use my existing different size cutting bits, correct?
> 
> Or are you suggesting a R8 ER32 chuck that only accepts 3/4” shanks?



Let me see if I can make this crystal clear.

Your spindle is an R8 spindle that accepts any R8-shaped shank. This tool is held solidly in the spindle with your drawbar. As the drawbar is tightened, it pulls the R8 shank up into the spindle and holds it solidly. If the thing you are placing in the spindle is a solid shank, like a chuck with an R8 shank, then the drawbar simply holds that thing solidly in place. If the thing is an R8 collet then as the drawbar tightens it collapses the collet around whatever you put in the collet and that holds that tool solidly. Sorry to get so basic but I hope this removes the confusion.

An ER chuck has an R8 shank on one end and an ER chuck on the other, like this one from Glacern.




The R8 part is held solidly in the spindle of the mill by the drawbar and the ER chuck part now becomes the tool holding part of this assembly. ER collets have the same outside dimensions and shape but the holes inside the collet vary in size. When a collet is inserted into the chuck and the nut is tightened, it collapses the collet to solidly clamp whatever tool you inserted into the collet. An ER32 collet set typically allows you to clamp any round tool shank from 1/16" to 3/4". That is, any tool you have with a shank that falls somewhere in this range can be clamped in one of the collets. So, one chuck, many tools.

Some guys, especially the CNC guys and in most industrial applications, will use multiple ER chucks. Rather than change the tool in the chuck, they just change chucks. He might have a rouging end mill in one chuck and a finishing end mill in another chuck. Because the end mill sticks out a precise amount and since it takes time to set this stick out, it is simpler to just leave it in the chuck and buy another chuck to hold another end mill that will have its own degree of stick out. This allows the user to go from one operation, roughing, to another operation, finishing, very quickly by just changing chucks. I believe this is what @Boswell is alluding to.

This is not the norm for most hobby guys. We have one chuck and we change tools in that chuck by using the appropriately sized collet. One chuck that holds any tool within the clamping range of the collet set, and it will hold every tool solidly and accurately.


----------



## Downunder Bob (Jan 1, 2018)

And Happy New Year to you also. Just re-inforcing and consolidating what has already been said. Ok a 1" cutter is a bit big for your mill, 1/2" should be good , you might get away with 3/4" but I wouldn't push it any further.

Your mill has R8 pocket in quill, R8 collets are not as good as ER so get a R8 - ER 32 collet chuck will fit directly into your mill and allow you to use the best collet system around, Try to avoid the cheapest, but you don't have to buy the best either. You can get a R8 - ER 32 collet chuck with a full set of collets at quite reasonable prices.

Also if you have a lathe, it will most likely have a Morse Taper in the spindle bore, so you can also get a MT - ER 32 collet chuck to suit your lathe, thus using all your collets twice. ER collets are very good for holding small round stock in a lathe as well as mill cutters. In a lathe you can use this set up for horizontal milling. best of both worlds.


----------



## Geerbangr (Jan 2, 2018)

You guys are the best!! ER 32 collet system it is. I’m trying to buy tooling and learn the best or closest to the best way possible to do machining so when I step up to a Bridgeport mill I’ll be in respectable standings to use such machine. I’m just a car hobbyist that needs parts machines and or made from time to time and hate waiting to get work done at a shop.


----------



## Geerbangr (Jan 2, 2018)

Does 120.00 seem fair for a new Glacern ER32 R8 chuck? No collets, just the chuck.


----------



## mikey (Jan 2, 2018)

Have you seen this one?

https://www.ebay.com/itm/NEW-Glacer...877680?hash=item416b5921b0:g:z0IAAOSwq7JULjiW


----------



## Geerbangr (Jan 2, 2018)

Yes that’s the one I was looking at Mikey. It’ll be about 120.00 shipped. Does that price seem fair? I messaged the seller and there’s no wrench with the chuck. The wrench is 16.95 extra. I wanted to ask you guys if the price was fair then I’m going to see if they’ll combine items for shipping.


----------



## mikey (Jan 2, 2018)

Yeah, that price is fair. I do not own one but I will someday. The specs on the chuck are very, very good. If you use good collets (not cheap; good) in it, it will serve you well for many years. Spring for the wrench; you will need it.


----------



## Geerbangr (Jan 2, 2018)

Well I’m the owner of a Glacern chuck and wrench. 

Now I need to locate a set of collets that’ll work nicely with the chuck.


----------



## Geerbangr (Jan 3, 2018)

Would the Shars brand of ER32 collets be worth considering?


----------



## Mitch Alsup (Jan 3, 2018)

I am using and enjoying the R8-ER40 in my Mill. ER40 has 1" (25mm) capability while ER-32 stops at 0.8" (20mm).


----------



## ddickey (Jan 3, 2018)

I have ER40 collet that can hold up to 1.1875".


----------



## mikey (Jan 3, 2018)

I suggested an ER32 because this is a benchtop machine that in all probability will not use huge cutters.


----------



## mikey (Jan 3, 2018)

Geerbangr said:


> Would the Shars brand of ER32 collets be worth considering?



G, you may not get an answer to your question because it is buried in this thread. Why not post a new thread asking which collet sets the guys would recommend?


----------



## Downunder Bob (Jan 3, 2018)

Mitch Alsup said:


> I am using and enjoying the R8-ER40 in my Mill. ER40 has 1" (25mm) capability while ER-32 stops at 0.8" (20mm).


You don't say whaty size your mill is, As others have already said ER 32 is about the max practical size for his mill, so not much pioint wasting money on a larger, more expensive unit that he wouldn't or shouldn't be using on his mill'


----------



## Geerbangr (Jan 4, 2018)

Mikey and Bob, I ordered a set of Tecknics collets. I know these parts are mid grade tooling but I think they’ll serve my low grade self well.


----------



## Downunder Bob (Jan 4, 2018)

G'day Geerbangr, They should be quite good enough for what you are trying to acheive. we understand you're not trying to acheive toolroom standards, so why waste the money, I'm sure there are other things you would like to spend it on. Good luck and happy chip making. Don't forget to post up the results and comments on things you have learned on the way


----------



## Z2V (Jan 4, 2018)

Late to the party but Glacern sells their R8 ER32 chuck for $89.99 on their own website.


----------



## mikey (Jan 4, 2018)

Geerbangr said:


> Mikey and Bob, I ordered a set of Tecknics collets. I know these parts are mid grade tooling but I think they’ll serve my low grade self well.



Good choice, G.


----------



## Geerbangr (Jan 9, 2018)

I received my new goodies today. Haven’t had a chance to use them thou.


----------



## mikey (Jan 9, 2018)

Excellent choices, G! I know that cost you a bunch but an accurate ER chuck and collet set is money well spent.


----------



## Downunder Bob (Jan 10, 2018)

Geerbangr said:


> I received my new goodies today. Haven’t had a chance to use them thou.


Excellent, enjoy playing with your new toys and getting to know them.


----------



## Driveslayer45 (Jun 5, 2019)

This is an old thread but I am not sure I understand why an ER Collet chuck with Er collets in a R8 spindle is more accurate than an R8 Collet directly in the R8 spindle? seems to me you are tolerance stacking by adding the chuck into the R8 and then the collet into the chuck, then the tool into the collet... what do i not understand?


----------



## Jake2465 (Jun 5, 2019)

I believe it's more to do with increasing versatility of the R8 spindle. Also, That system has a locking nut on it, so one just has to hit the brake and take a spanner to the nut instead of reaching way up there on top of the head to get at the drawbar.


----------



## Mitch Alsup (Jun 5, 2019)

Driveslayer45 said:


> what do i not understand?



There are other holders (like 4 sided and 6 sided collet holders) that can use these same ER-40 collets.
Whereas there are no 4-sided and 6-sided collet holders for R8
Whereas there are 4-sided and 6-sided holders for 5C collets.

However, that said, and the fact I actually have such an ER-40 holder in R8::
I have come to the conclusion that it is better just to buy R8 collets for the R-8 spindle
for 2 reasons
a) nore nose height to table
b) less tolerance stackup;
cost be damned....


----------



## mikey (Jun 5, 2019)

I'll take a stab at this. If you have good R8 collets, like Hardinge collets that have a confirmed run out of 0.0002", then you are  contending with the fact that R8 collets grab the tool shank with only about a 1/2" of surface area, much like a C5 collet, and the fact that the tool shank must be within about 0.005" of the collet size to be held solidly. Good R8 collets are quite accurate; junk collets are not.

An ER collet system has several advantages. It grabs the tool over a longer surface area so it registers the tool more accurately inside the collet. Due to the geometry of the ER design, it surrounds and clamps the tool shank very solidly. If you have an accurate chuck and use good collets then run out is minimized. Moreover, an ER system dampens vibration better due to the mass of the chuck/collet/nut system. Finally, a good ER system is very accurate over a wider range if the chuck is good, the collets are of good quality and you use a good nut that is torqued properly. Granted, the collet is most accurate when used with a tool shank very close to its stated size but small variations in tool shank size can be easily accommodated. 

One of the key reasons that ER collets are a standard in the industry is because rather than change the tool in the chuck, the entire chuck is changed when a tool change is needed. Tools are locked into the chuck and remain there unless it wears. Imagine if you had to completely unscrew a draw bar, change out an R8 collet, change out the tool and then screw in the drawbar again to lock the new tool in. Very cumbersome. 

I use the Tormach TTS system and have several ER chucks. It is very fast to swap out one ER chuck for another when multiple tools are needed. I think you can go either way in a hobby shop but for me, the ER system has enough advantages that I prefer it over R8.


----------



## Titanium Knurler (Jun 6, 2019)

mikey said:


> Just one more thing. ER collets are often used on the lathe for work holding and do an adequate job of it. However, run out on the lathe is not nearly as critical and you can get away with an import collet set. On the mill, accuracy counts and there I recommend you suck it up and buy a decent set of collets. It will cost you but you will recover the cost over time because your tooling will be more accurate and will last longer.



Mikey, a newbie question:  I believe I understand that with _tool_ holding the run out is important for accuracy and tool wear reasons but why is accuracy not as critical with _work_ holding?


----------



## mikey (Jun 6, 2019)

Titanium Knurler said:


> Mikey, a newbie question:  I believe I understand that with _tool_ holding the run out is important for accuracy and tool wear reasons but why is accuracy not as critical with _work_ holding?



A fair question, and I'm sure others have their own opinions. There is no reason you cannot use high quality collets on the lathe. The reasons I don't feel the expense is justified are:

Most of the stock we use in these collets can vary greatly in size. As you know, the farther away from the stated size of the collet the less accurate the collet becomes. Granted, this is less of an issue with higher quality collets but it occurs with all of them.
Most of the time, we do not need to work to tenths level tolerances on the lathe. Not only do we not need to do that but you have to ask yourself if you can work to those tolerances. If you use a good nut, you can get a cheap Chinese collet to run out under a thou easily. In fact, with an ETM nut I can get my cheap collets to run out close to 0.0004" TIR, which is 0.0002" actual run out. How much more accurate do you need to get? Can you cut anywhere close to those tolerances with an inserted carbide tool? Really? I can do it with a well-ground sharp HSS tool but with carbide and the deflection I get from the nose radius, that is a challenge.
Truth be told, when I have a critical dimension to hit, I don't use a collet. I use my 4 jaw chuck and I dial it to zero, and then I cut it with a HSS tool. I actually don't use collet chucks often. I use them when I do not wish to mar a fine surface on a previously turn work piece. I use them if the work piece is threaded and I'm trying to avoid damaging the threads, and I use collet chucks when working up close to the chuck with my hands. Otherwise, I use a jawed chuck.


----------



## Titanium Knurler (Jun 6, 2019)

Mikey, all makes good sense, Thank you, TK


----------



## rock_breaker (Jun 7, 2019)

Geerbangr,    You mentioned "home on leave" If you are in the military I would like to thank you for your service. Otherwise thanks for being a member here.
Ray


----------

