[ihavenofish]

Thanks leggazoid...that looks very much like what I am looking for.

that machine is $4000 over your budget, and is no more precise than the tormach and novakon nm200. it uses the same steppers, same grade ball screws, same control software, has same overall rigidity range.

there was actually something cool that would have suited you for sale up here in canada a while back. it was a brother tapping centre. a pair actually for $6300. these are old low power micro VMC's complete with tool changer and high precision and performance that would have retailed for $40k or so new. the reason they sell so cheaply now is they only offer tapping and drilling and very basic 2d linear motion. they also only have 8"x11" travel. spindles were 6000rpm and 2kw if i recall.

you would swap out the control for a PC running emc2 and off you go with full 3d contouring abilities. a few people on the forum have done this and they work well. could probabaly have both machines with some tools running for under $10k.

[Rockn-Roll]

I just received the machine precision specification from Tormach...apparently they have it posted on their web site at Certification of Inspection. Apparently every Tormach which is sold has those tests performed and the actual measurements noted. It's not ISO 230, but at least it is test results.

The allowable positioning precision of their PCNC 1100 is .03" and the resetting precision is .02". I'm sure if I measured each axis movement and manually corrected it then I could use their machine to come within .001"; however, the whole point of having a CNC machine is so that it will happen automatically. Greg Jackson at Tormach has indicated that their machines will not meet my needs.

Does anyone know where I can find similar specifications for some of the other machines in my price range? I'm currently sending requests for something of this kind from other manufacturers. It sure would speed up my decision making if I could see some actual machine specs such as what Tormach is providing.

[ihavenofish]

I just received the machine precision specification from Tormach...apparently they have it posted on their web site at Certification of Inspection. Apparently every Tormach which is sold has those tests performed and the actual measurements noted. It's not ISO 230, but at least it is test results.

The allowable positioning precision of their PCNC 1100 is .03" and the resetting precision is .02". I'm sure if I measured each axis movement and manually corrected it then I could use their machine to come within .001"; however, the whole point of having a CNC machine is so that it will happen automatically. Greg Jackson at Tormach has indicated that their machines will not meet my needs.

Does anyone know where I can find similar specifications for some of the other machines in my price range? I'm currently sending requests for something of this kind from other manufacturers. It sure would speed up my decision making if I could see some actual machine specs such as what Tormach is providing.

i think youve scrambled your units. the tormachs positioning should be .03MM and repeatable to .02MM, or .0008".

that sounds about right, in terms of basic ball screw positioning. you still have everything else to contend with in the machine, tool, fixture, part, and human factor however. you main problem will be the repeatability, which is difficult to compensate for with a good setup.

as ive said, even DMG will only quote .0004" precision on a standard ball screw machine, and they are "the best money can buy".

there was an interesting thread here a while back from someone with a haas machine. he ran a cut, had the machine stop in the middle, then continue. at the "stop", the force from decelleration made the whole machine bounce and left a small but measurable divot in the work piece. just some extra insight into the intricacies of making something precise.

[arizonavideo]

My father in law was over tonight for dinner and he is ready to get his retirement in March from the machine shop he has been at for the last 20 years. It is his second retirement, his first one was from FMC. That's 40 years of machining.

He is a tool maker and makes mainly high spec aircraft and military parts.

I placed a motor mount in front of him and asked what it would take to make this part to +/-.0005" in all dimensions. His answer was "you cant"

If you have a part you can't hold .001" all over without the expense going through the roof. No mater what you will junk more stock or have to have some surfaces built up. Just the cost to measure it would be silly to all but the vary rich.

If you have to hold .001" on a single operation on one or two surfaces and the rest .004 then it becomes something that many shops can make or even a home shop.

Cut the part and send it out to be ground is a standard way of doing things to hold .001" or better on a few surfaces. Did they skip that in school?

If you start talking about surface tension and such a shop can relieve and treat a part for a few K more....

You never described you real needs just a spec that can't be met by any hobby machine.

It is a bit hard to tell if you are even serious about the question with the lack of detail of the part.

If you care to learn the Tormach is a fine machine and a good place to start to make parts. Resale is good on the smaller mills so the risk is small. The Novakon NM-200 looks great too I just haven't heard much from users.

If you don't want to learn how to make parts then buy the imaginary machine that will hold +/-.0005" in all dimension for 10K, I hear their is no back order on them.

[GITERDUN]

You never described you real needs just a spec that can't be met by any hobby machine.

It is a bit hard to tell if you are even serious about the question with the lack of detail of the part.


If you don't want to learn how to make parts then buy the imaginary machine that will hold +/-.0005" in all dimension for 10K, I hear their is no back order on them.

Can you imagine the frustration of all those poor tool salesmen as they spend countless hours on their toll free lines trying to explain to this guy why he can't build his Mars rocket with a Harbor Freight 3 in 1.

[Rockn-Roll]

Some of you are purposefully exaggerating my needs. Only a few of you are being resonable. If you absolutely need an example part and the required tolerance in order to understand what I need then fine...I'll give you a sample part...all the way from raw material to how I will measure the precision.

Material: 1018 Cold Rolled Steel.
Online Reference: Metal Express - Error

Tool: 1/4" diameter End Mill with Ball End.
Online Reference: http://www.shopatcdirect.com/default...rbide+Ball+End

Starting Blank: 1' long Square Bar Stock with cross-section: 5"x5"
Milling Process: Bore a 1.5" +.01" deep square hole with cross-section of 1.690"x1.690" +/.0005" tolerance for cross-section dimensions (1/4" fillets at all internal edges and corners). Location of hole is 2.5" +/-.005" from one edge of the bar (doesn't matter which side) and 2.0" +.01" from the end.

Starting Blank: 1" Square Bar Stock with cross-section: 1-3/4"x1-3/4"
Milling Process: Remove approx. .059" from two adjacent sides so that the resulting bar has a cross-section of 1.691"x1.691" +/.0005" (1/4" fillets at all external edges and corners)

Note: The resulting finished products will be a square hole with cross-section no smaller than 1.6895"x1.6895" and no larger than 1.6905"x1.6905" and a square bar with cross-section no larger than 1.6905"x1.6905" and no smaller than 1.6915"x1.6915". The design requires that the square bar should fit into the square hole with an interference fit of no less than 0.0000" and no more than .0020". The final assembly will be a 1' long 5"x5" square Steel armature with a 10-1/2" long 1-3/4"x1-3/4" shaft sticking out of it at a 90º +/-.01º angle. The tolerance for the position at the end of the 10-1/2" long shaft needs to be +/-.002" in order to minimize, within reason, the internal stresses.

Initial measurement of the finished products will be made using a dial guage vernial caliper with inside/outside jaws and a precision of +/-.00025". Final measurement of the finished products will be made by heating up the 5"x5" bar stock containing the hole until the bar still at room temperature fits by hand into the hole. The Coeff. of linear expansion will be determined by experimentation using a dial-gage vernial caliper with precision of +/-.00025" and an infrared heat gun with precision of +/-1ºC (expected value will be approx. 15x10-6/ºC). I expect the bar containing the hole will need to be heated to about 155ºC using a propane heater rated at 85,000 BTU/hr. If it needs to be heated more than the expected maximum then the interference will be more than my design allows...and if it doesn't need to be heated at all then it will not be an interference and the shaft will not be centered in the hole and will exhibit movement and deflection with very little force. This isn't rocket science.

It is crucial that the interference fit be no less than .000" and no more than .002"...hence my initial requirement that the precision of each cut be no more than .001" (+/-.0005" if you wish). I'd also like to point out that using an infrared heat gun with 1ºC of precision provides me with the ability to adjust the dimensions of the 1.690" hole in increments of .000025" (1.690" times 15x10-6)...I'm just trying to get the initial room temperature measurements within a reasonable tolerance. I can modify the measurements of my parts by controlling their temperatures to get them within +/- .0001" if I need to.

The products that I'm going to make don't currently exist, so I can design them anyway they need to be designed. If a product needs the parts to be kept at a constant temperature differential (+/-1ºC) in order to maintain dimensions then that's what I'll have to design...that's my job as an engineer to determine what the parts need to be and how to use them. All I'm asking from machinists here is what CNC machine tools are available for $10,000 that can position a part with +/.0005" precision and have a 2HP spindle motor. If none exist for $10,000 then that's what I will learn and I can increase my budget.

[ihavenofish]

a few things.

1018 cold rolled will warp alot (.1" or more) if you cut a pocket that big out of it in one operation. not an ideal material for the task. if you must use 1018, youll need to rough the pocket, stress relieve, re rough, then do a finish pass.

with a 1/4" end mill and 1.5" tall walls, you will not get a squared pocket easily. id increase the tool diametre to 1/2" or more.

fitting 2 parts together like that will be tricky. youd really want to mill the pocket, measure its actual size accurately including out of squareness and taper. then mill the insert oversize, measure it, then grind it to final size.

likewise getting the hole within .005" of the edge will require several stages of roughing and possibly grinding that edge before and after the main pocket is finished.

basically, any machine with no backlash and good rigidity will do this part, because the limiting factors are not the machine.

[skullworks]

Some of you are purposefully exaggerating my needs. Only a few of you are being resonable. If you absolutely need an example part and the required tolerance in order to understand what I need then fine...I'll give you a sample part...all the way from raw material to how I will measure the precision.

Allow me to point out how and where you have failed to consider what your needs truly are.

Material: 1018 Cold Rolled Steel.
Online Reference: Metal Express - Error

Tool: 1/4" diameter End Mill with Ball End.
Online Reference: http://www.shopatcdirect.com/default...rbide+Ball+End

Why are we using a 1/4" dia. tool in a 1.5" deep pocket? Proper engineering choice would be a 12mm tool or even a 12.5mm which will still allow your 1/4" fillets and still have some rigidity.

Starting Blank: 1' long Square Bar Stock with cross-section: 5"x5"
Milling Process: Bore a 1.5" +.01" deep square hole with cross-section of 1.690"x1.690" +/.0005" tolerance for cross-section dimensions (1/4" fillets at all internal edges and corners). Location of hole is 2.5" +/-.005" from one edge of the bar (doesn't matter which side) and 2.0" +.01" from the end.

Now if your pocket was all the way through you could wire EDM the pocket and hold the numbers your asking. But its not and there are fillets between the walls and floor. The length of the straight wall above the fillet is about 1.25". Your Dial Calipers will allow you to measure perhaps the top .5" but most likely there will be a taper in the wall so you will not know the true width just above the fillet.

Starting Blank: 1" Square Bar Stock with cross-section: 1-3/4"x1-3/4"
Milling Process: Remove approx. .059" from two adjacent sides so that the resulting bar has a cross-section of 1.691"x1.691" +/.0005" (1/4" fillets at all external edges and corners)

Note: The resulting finished products will be a square hole with cross-section no smaller than 1.6895"x1.6895" and no larger than 1.6905"x1.6905" and a square bar with cross-section no larger than 1.6905"x1.6905" and no smaller than 1.6915"x1.6915". The design requires that the square bar should fit into the square hole with an interference fit of no less than 0.0000" and no more than .0020". The final assembly will be a 1' long 5"x5" square Steel armature with a 10-1/2" long 1-3/4"x1-3/4" shaft sticking out of it at a 90º +/-.01º angle. The tolerance for the position at the end of the 10-1/2" long shaft needs to be +/-.002" in order to minimize, within reason, the internal stresses.

Initial measurement of the finished products will be made using a dial guage vernial caliper with inside/outside jaws and a precision of +/-.00025". Final measurement of the finished products will be made by heating up the 5"x5" bar stock containing the hole until the bar still at room temperature fits by hand into the hole. The Coeff. of linear expansion will be determined by experimentation using a dial-gage vernial caliper with precision of +/-.00025" and an infrared heat gun with precision of +/-1ºC (expected value will be approx. 15x10-6/ºC). I expect the bar containing the hole will need to be heated to about 155ºC using a propane heater rated at 85,000 BTU/hr. If it needs to be heated more than the expected maximum then the interference will be more than my design allows...and if it doesn't need to be heated at all then it will not be an interference and the shaft will not be centered in the hole and will exhibit movement and deflection with very little force. This isn't rocket science.

Dial gage Vernier Calipers - Are you serious? First off you need a stopwatch and a heat sink to re-stabilize them because the amount of error grows for every second its in your hand. For measuring the block a good tenth reading micrometer would be better suited to the task.

It is crucial that the interference fit be no less than .000" and no more than .002"...hence my initial requirement that the precision of each cut be no more than .001" (+/-.0005" if you wish). I'd also like to point out that using an infrared heat gun with 1ºC of precision provides me with the ability to adjust the dimensions of the 1.690" hole in increments of .000025" (1.690" times 15x10-6)...I'm just trying to get the initial room temperature measurements within a reasonable tolerance. I can modify the measurements of my parts by controlling their temperatures to get them within +/- .0001" if I need to.

The products that I'm going to make don't currently exist, so I can design them anyway they need to be designed. If a product needs the parts to be kept at a constant temperature differential (+/-1ºC) in order to maintain dimensions then that's what I'll have to design...that's my job as an engineer to determine what the parts need to be and how to use them. All I'm asking from machinists here is what CNC machine tools are available for $10,000 that can position a part with +/.0005" precision and have a 2HP spindle motor. If none exist for $10,000 then that's what I will learn and I can increase my budget.

The pocket you want - even on a Million Dollar plus Mori Seiki will come down to matching coolants, tool materials and coatings, tool holder optimization, tool loading machining strategies, and a series of in process inspection to come near making your part.

Rocket Science, nope. Rockets are easier.

You appear to have thought it through, problem is you seem to have over looked something between the lines, every other line as may be.

Now for your block - have you considered a granite surface plate and emery cloth to finish lap your block to spec... dirt cheap - but it puts the skill in the operators hands and outside of the machine.

[skullworks]

There is a 99% chance the OP design is way over complicated for what the actual needs are.

:violin:

NASA spent millions making a ball point pen that could write in any orientation in zero gravity.

The Russian space program just used pencils.

I used to make a small fortune redesigning parts for reduced cost of manufacture.

Then a US computer corp offered me alot of money, a nice desk with air conditioning, free coffee (delivered to my desk) no worriers when I was off the clock, and the heaviest thing I had to lift all day was a mouse (coffee mug was optional).

I'm still an IT Admin as my day job, that Hurco CNC in my garage is there to allow me my creative fix when I just have to make some new toy.

[Rockn-Roll]

Thanks for posting, but again...keep in mind what the topic is. I'm trying to focus this thread on the availability of machine tools...not any particular part or material. I provided a sample part for the sake of pointing out the dimensions and tolerance of a sample part and how I might measure it. If I don't like the machinability or milled finish of a specific material then I can use another one.

I am looking for a CNC machine with which when I tell it to position a cutting tool the machine will be within +/-.0005" of that position.

As for the Tormach specs...yeah, I'm definitely wrong there...it says millimeters. According to the G8 and G9 spec it looks like the machine should be able to move to a position within .03mm (+/-.0012") of where I tell it and then repeat it within .02mm (+/-.0008")...a total of .05mm (+/-.002"). This does agree with the precision that Tormach gave me in the emails. While it is possible that the actual machine that is delivered has the necessary +/-.0005" precision...it also looks like it's possible that I would get a machine that has +/-.002" precision. I do admit that the Tormach comes close, but not close enough to risk $10,000 on it. I'd rather spend $20,000 or more on a machine that meets my requirements than spend $10,000 on a machine with which I cannot make the parts that I want to make.

[thedave]

I hope this helps.

What you are asking for can't be accurately answered without a specific application of said machine tool. It would be like someone asking you if you could install a Gigabit network for $ 10,000. no other details.

The truth is machine positioning is the easy part. Material type, work holding, machine rigidity, tool material, tool length, speeds, feeds, ect... all contribute to the machining equation. When machining, everything flexes, all the way down to the tool itself. The question you should be asking is, "I want to build X, what is required to do that". Otherwise you are just chasing specs, and you can get those from the manufacturers and put that into a spread sheet.

[Rockn-Roll]

Otherwise you are just chasing specs, and you can get those from the manufacturers and put that into a spread sheet.

That's exactly what I'm trying to do...find the specs. Most manufacturers don't provide those specs...some don't provide any number for their precision and allude to vague descriptions of how close their tolerances are when they assemble the machines. Sometimes a manufacturer will quote different numbers for the same spec depending on what salesman you talk to. Some manufacturers have the specs, but the machines that they deliver have an "actual" measured precision which is way outside of the machine's advertised spec. Some only measure one machine out of 10...so no matter what the papers say...the machine that is delivered could be out-of-spec.

I'd like to avoid finding out that a machine doesn't have a positioning tolerance of +/-.0005" after the machine is delivered...it will save me about a thousand dollars in shipping charges if I find out what the precision of the machine is "before" I plug it in and measure it's performance.

Also, by my specifying a single criteria i.e. positioning, I eliminate all the other variables. My point is that if the machine cannot position a cutting tool within +/-.0005" then none of the other criteria makes any difference to me. I'm only going to look at the other criteria i.e. rigidity, paralallism, etc. if the machine has a positioning precision of +/-.0005". This may not be how other people do it, but it's how I'm doing it.

Please stick to the one and only criteria that I'm asking about otherwise this thread will be filled with vague discussions on machinist skills and how machine deficiencies can be overcome, heated debates on the effects of tool and workpiece temperatures on the machine precision, etc like some members persist in doing (i.e. it's too late but I hope to prevent the thread from straying too far too often).

As I pointed out the Tormach machines come close...repeatability of +/-.02mm (.0008") and positioning +/-.03mm (.0012"), but obviously this is not +/-0.0005" and this will also be effected by the machine's parallelism spec and any lack of rigidity under cutting loads. Parts made with a machine delivered with these precisions most likely will only be within +/-.002" at best, and most parts require 2 cuts (one on each side of a dimensioned section) so it's more than likely that the average tolerance of a milled part would be something like +/-.003". I've done my share of grinding, honing, lapping, and polishing to achieve the required dimensions of parts after using my hand tools to remove as much as I dare to know that I can perform additional manufacturing processes to achieve a precision down to 0.0001" if I need to, but that's not the point of this thread. I'm aware of the additional processes and what I'm saying is that I won't need them, or at least I can minimize their need, if the machine has a precision of +/-.0005". But, I have not had the money to purchase a machine tool before so I never looked at them other than in my dreams. I assume that some of the members here at CNCzone have a machine tool or at least know a lot more about them than I do. And, thankfully some are willing to share...even more than what I need.

I admit that the "more than I need" posts are frustrating me, and initially I did suspect some of you as being trolls (no paid membership, exaggerating what I'm saying, straying off topic, etc.). But, based on the responses from other members and the forum admin it seems that you are all genuine, so you have my hearty thanks for posting and helping me out especially since it may appear that I'm completely mis-guided. So, the following is perhaps a good read to see that my requirements are well founded and based on a reliable source:

According to the Machinery's Handbook section on "Allowances and Tolerances for Fits" (in the 28th edition it starts on page 627) the Tormach would not be a machine that could safely produce interference fit parts. The parts might just slip off or the internal stresses might be too much and the hub will break during assembly or worse when the part is put into service. I highly recommend anyone participating in this discussing read that section and understand why I'm looking for a machine that has a positioning precision of +/-.0005" and why that is the main criteria for a machine that I would be willing to purchase.

A good example is in the Dimensioning, Gaging, and Measuring section...the first sentence of the paragraph titled, "Allowance for Forced Fits" on page 629 which says, "The allowance per inch of diameter usually ranges from 0.001 inch to 0.0025 inch, 0.0015 being a fair average." But, more specificially is Table 11 for ANSI Standard Force and Shrink Fits (page 645 of the Handbook or page 290 of pocket companion). Most of my interference fits will use 1/2" through 3/4" dowels which means the row I need to look at is where Nominal Size Range, Inches is 0.056 - 0.071. The amount of pressure/torque I will be looking for requires a class FN 4 fit with H7/u6 material Interference of 0.7 / 1.8 which requires a precision of 1.8 - 0.7 = 1.1 thousands. In other words, if I designed the parts so that they are machined for an interference fit of 0.00125" on a machine tool with precision of +/-0.00055" then I would not loose any sleep over it. For example in a production run I could just measure a sampling of the parts at regular intervals to maintain quality control and not worry about having to scrap any of them unless there's an operator error of some kind or something has really gone wrong.

But, if those same parts are machined on a machine tool with a precision that is greater than +/-0.00125" then I could wind up with an interference fit of .00125 - .00125 <= -0.0" i.e. the parts would just slip off. All the parts would require a redesign and post-milling operations will be needed to bring the parts within tolerance and hence be labor intensive. If I was going to keep up with my typical grinding, lapping, and polishing practices then I would just buy a drill press. Fortunately, I have enough money to spend on a machine that is more advanced than a drill press i.e. a mill. I started my seaching looking at drill presses then I looked at 3-in-1 mill/drill/lathe machines and then dedicated vertical mills, and finally CNC vertical mills. Anything will be better than my hand drill and dremel drilling station.

As I progressed through my searches I found that the precision of the machines increased along with the price. From some of the web sites it appeared that the precision of the machines were approaching .001" as the price was approaching $10,000. After the $10,000 machines, though, the price seems to jump all the way to around $40,000 and have a precision of 0.0001" along with way more horsepower and features than what I need i.e. production machines. I don't have the budget for a $40,000 machine, but perhaps something in between might work...that I can finance the rest. I don't know, but I hope there is...and eventually I believe this thread will reveal at least one that meets my needs.

Thanks

[DareBee]

Well said.

I am afraid you will have to compromise and buy a machine like the Tormach, MN or Mikini.
This machine [nomedia="http://www.youtube.com/watch?v=ISzkthutKnA"]YouTube - Scratch Built mini version of Fadal&#39;s VMC 15[/nomedia] is VERY impressive. No idea what the specs are and likely costs 30+ thousand (but you won't know unless you ask).
Best of luck in your continued search.

[eded59]

I think you're limiting yourself by ruling out used machines
BRIDGEPORT SERIES II RIGID RAM INTERACT-2 CNC MILL - eBay (item 220625537768 end time Apr-16-11 15:24:12 PDT)
I would much rather start with something similar to this if it was up to me to make this part as opposed to any of the machines you are looking at. Even with a rotary phase converter your money ahead. Most problems with older equipment is in the electronics, and it sounds like you have that covered..

[pete from TN]

This is quite a thread here. I have read down thru it and my head hurts!! The poster apparently is a well educated man. He is also according to his own words versed in machining while in a mechanical engineering study program. However his posts are quite vague and despite the efforts of some pretty knowledgeable fellows on here he takes the stance that people are attacking or trolling him. This is not what I read here. I know you feel like people are skirting your issues and trying to make you feel like you are not asking the right questions. The reality is that they are trying to help you....

I have NO engineering degree. I have been manually machining parts for over a decade. I recently build my own CNC milling machine retrofit. I also have NO idea what you are trying to build or what kinda precision or stresses you intend to put these parts under. What I can tell you is that I cannot afford a precision high end machining center, I wish I could but that is really the realm of professional machinists that have products and contracts that can pay for the machines. In fact for most shops like that the cost of the machines is negligible over the amount of money they make and the products they sell. It is beyond most here to be able to operate in that realm and these people spend more on tooling every day than you wish to spend on the whole machine.

This is not to say that what you are looking for is impossible. Quite the contrary.... Let me explain. I have an asian lathe here that is halfway decent. It has dials that can indicate to .001 and I can extrapolate more precision than that where necessary. Despite the fact that it is really only as accurate as the dials can show I have built precision airguns that carry 3000 psi of air pressure safely inside it and cut O-ring grooves and pressure tested the vessels myself. I have also made precision sliding and friction fits that work quite well if I am careful.

MY milling machine is an RF45 CNC mill that I converted from a manual machine. It is similar in size and capacity to the Tormach machine. I use it to make all sorts of parts and when I NEED To I can attain some nice accuracy often to .001 or .o02. However there are situations where the accuracy of a part needs to be REALLY tight. Specifically hole sizes and depths. This is when I usually mill out the pocket close and then use my boring head or a reamer to finish to a precise size. It has been said that a good machinist can make accurate parts on an inaccurate machine. This is ABSOLUTELY true. I however am not a GOOD machinist. I am however a stubborn bastard and will fight and futz with it until I get what I need out of it.

If what you are making has very precise milled slots or holes in certain areas then you can do a lot of things to make those parts work. Let's say you do some Cad and Cam work and generate some code for this phantom part. Then let's say you need to make say twenty of them. Well you put your metal in the machine, hit go, watch and make sure it does what you want it to, and then take it over to your nice accurate granite surface plate and matching height gauge. You measure carefully your part and realize that well hell it is not good enough here or there. Part of the beauty of CNC is just that it will do EXACTLY what you want it to and nothing more. SO you can take your part, record the areas where the numbers are not working and go back to your cam software and make some adjustments for the length or width of those machining operations or even just cheat the machine and tell it the cutter is not as big or as small as it thinks and then re=run the part. This may take a time or two to get it right but in the end your less than perfect milling machine CAN make accurate parts. It is just a matter of tweaking stuff.

Now don't let me kid you here. This is NOT simple and easy nor is it cut and dry. The reality is that if you only have manual machining experience it will take quite a while learning making wrong parts before you get the hang of it and start making accurate parts. If you have NO manual machining experience then you are really in for an adventure. I have some good friends here in Tennessee who operate a very high quality CNC job shop. They have brand new mills there and some older high quality mills there too. I often go there and talk to them about machining and try to learn as much as I can from them. Believe me when I tell you that there is NO such thing as a machine that you just plug in numbers and it spits out a perfect accurate part. Even with their mega bucks machinery and state of the art tooling they still have to often tweak their code to get the parts accuracy they need. The reality too is that even for them MOST parts only need to be REALLY precise in a couple areas not usually the whole part... It is just not the way of things. I have watched them make some rather incredible and beautiful stuff for all manner of industries and believe me they know what the hell they are doing. In fact the business is a family business and the great grandfather stared it years ago with manual machines and now they have some wicked CNC stuff and laser machines, plasma cncs, multi axis CNC lathes and enough machining centers to fill a wal mart. Getting accuracy out of a machine regardless of price is a delicate balancing act. For someone like yourself that may mean balancing to try to eek out the tolerances you need for that part on your sub $10k machine, for them it is eeking out that really precise part all while making ten thousand of them in a week or something. It is what machinists do, it is literally what makes a machinist a machinist!!

If I were you I would cease laboring over tech sheets and number crunching and step back a minute, Ask yourself what you really want from the machine and what you need it to do and then choose a machine that is adequate for that purpose. Honestly if I were in your shoes, I would be looking at a used machining center that you can run on a phase converter in your home shop. I really like the Fadal's and there are some that would easily be in your range and can fit inside a small shop space. They will also allow you some production abilities if you intend to go that route in the future. Most importantly they are PROFESSIONAL machines made in the USA and were designed to run and run and produce accurate parts. There simply is not a chinese turnkey mill anywhere that will outperform one of these machines. You are apparently out in california and there is a TON of nice used machines out there for sale constantly. I used to live in Sacto and for buying a machine tool that area is the place to be. I would HIGHLY recommend you contact a used machinery dealer out there, tell him what you want and what you wish to spend and have him work for you to find it. These machines have much better spindles, they have toolchangers, they have much better travels and speeds and are just as I said built to last....

I wish you the best of luck finding what you are looking for here, I would also caution you to try to understand that everything is not cut and dry when it comes to machining. Yes there are lots of things that are but you would do well to open your mind to the ideas that others on here have posted about. They are actually making things with machines like this and have experiences that you do not have. That is a very valuable thing for you to take full advantage of. You would also do well to visit some local machine shops. Ask questions and LISTEN to what they tell you. People that really know what they are talking about when it comes to this stuff are usually willing to help a newcomer. That is right up until you start to tell them they do not know what they are talking about and then you will get a swift ushering out the door or worse a punch in the face.... Be courteous, be kind, listen to what they tell you, read all that you can about this extremely interesting topic and take your time. It is not beyond you as you are obviously a smart fellow. It just seems that you are upset that people have keyed on to your lack of machining knowledge based on what you have said in this thread. Nothing wrong with not knowing, but if you decide you know better than those that do well that is when you loose and the conversation takes a nosedive... Good luck to you and if you need any specific questions answered I will try to help you however I can. Peace


Pete

[BBchevy396_]

eventually I believe this thread will reveal at least one that meets my needs.

I believe everyone already knows what this thread has revealed.

[Rockn-Roll]

I ordered some Mitutoyo gage blocks and a 12-pc set of Fowler micrometers so I can measure outside dimensions from 0 to 12" with +/-.0001" accuracy. For inside dimensions I have ordered a 6-pc set of Fowler telescoping bore gages good for measurements of 5/16" up to 6"...I know I won't be getting anything better than +/-.001", but as I mentioned in my sample part...there are much more precise ways to measure internal dimensions if I need the extra accuracy.

The accessory that I'm currently shopping for is a level. I need to decide whether to get a double laser level system or a simple, but precise, 2-vial spirit level setup, or both. The fowler Cross Spirit Level is good for a gradient of +/-.001" per 10" and costs $610...the laser levels are cheaper, but I think it would be wise to have both. With the spirit level I can ensure very close tolerances on angles while the laser level will ensure consistent alignments between parts and sections of the same part. If I do decide to go with a used machine then I definitely will want to check the machine for parallelism...for which the levels would be useful.

[Delw]

I ordered some Mitutoyo gage blocks and a 12-pc set of Fowler micrometers so I can measure outside dimensions from 0 to 12" with +/-.0001" accuracy. For inside dimensions I have ordered a 6-pc set of Fowler telescoping bore gages good for measurements of 5/16" up to 6"...I know I won't be getting anything better than +/-.001", but as I mentioned in my sample part...there are much more precise ways to measure internal dimensions if I need the extra accuracy.

The accessory that I'm currently shopping for is a level. I need to decide whether to get a double laser level system or a simple, but precise, 2-vial spirit level setup, or both. The fowler Cross Spirit Level is good for a gradient of +/-.001" per 10" and costs $610...the laser levels are cheaper, but I think it would be wise to have both. With the spirit level I can ensure very close tolerances on angles while the laser level will ensure consistent alignments between parts and sections of the same part. If I do decide to go with a used machine then I definitely will want to check the machine for parallelism...for which the levels would be useful.

Telescopic gages, there only good for experianced machinest,and in my Opinion they should NOT be used for inspection only reference like a pair of calipers. very few people can use them and get a good dim. the longer the bore the less of an accurate reading your going to get. Dial bores are the ONLY way to go for inspection.

as far as checking parallelism on a used machine, fat chance unless its in your shop and powered up. parallelism is going to be dictated by level, which means your going to have to level the machine first, run it a few times then check the level again after it settles. I dont know anyone that would let someone come into there shop and let them level a machine run it level it then start checking it. besides you can adjust parallelism by tweaking a few things.

if you check anything the only thing you really need to check is backlash( after listening for normal items) then you need to compare that backlash you get get with the parameters on the machine to figure out if someone add'd too much or too little into the parameters. thats causeing the back lash.
on top of that there is straps and gibbs that can be adjusted on box way machines.
Frankly your wasting your time and money, and the sellers time for what your planning, Not trying to sound mean, but your clueless on machines and machining , how they work and what they are capable of.

your best bet is to HIRE someone to go take a look at the machine and let them give you there opinion of that said machine. if they say the machine will do what the machine is made to do then your good to go. however that doesnt mean the machine will do what YOU WANT IT to do. as again your clueless to what machineing is.
if you start yaking like you have in this thread sellers and machine sales people are going to tell you your a NUTJOB in nice terms, some sellers will tell you to go blow a goat, I know I would cause I think your nuts.
You havent listened to a single person on this forum thats trying to tell you the way it is in REAL life VS your fantasy.

I still think your full of BS when you say you sent parts out and every machine shop did them WRONG. if the shops were legit, then you screwed up in your design, LEGIT SHOPS CAN HOLD TOLORANCE, certain tol's. come with a price.
so in a NUTSHELL your trying to be a pratt and whiney on a $10,000 budget.


Delw