Machining of cast iron

Are you running a cooling mist on it while machining?

I would suppose you are doing production runs and the heat may be causing it, but .02mm to .05mm is a lot of difference. Almost as if it has to be in the 2nd setup.

But I'm sure you have dial indicated the chuck facings you are placing the 1st machined side against, correct?

Almost sounds as if the chuck is off by .01mm of parallel.

Hi !!!

Please also check movement of the slide while facing the plate is perpendicular to the axis of rotation of Spindle / chuck.

If it is incoorect you would generate eithera concave or convex face depending on the direction of error in squareness of movement.

Simpler method is to check the flatnes first and it should be less than 0.02 mm . see the flatness error for opposite face also. You would certainly get startling information if error in parallelisam is 0.04 mm.

Better consult some expert to check the accuracy of CNC Machine with the help of Renisha Ball bar and coorect the error if required after the test.

Udayan

Contact if required

udayan121049@yahoo.co.in

X & Z axis of the slide are less than 0.005mm.

4 jaw chuck has been using for both the operations.

As you said Flatness in the First operation is 0.02mm and to reduce it plz. provide a solution. Whether, the intermediate cut while facing might be a reason for the flatness to be 0.02mm.

Speed in the First & second operation, is min.500rpm to max.1000rpm and feed 0.08mm/revolution.

During facing operation(second operation), i also found that parallelism towards the center reduces from 0.04 to 0.00mm.

Yes sir, coolant(oil mixed with water) has been used while machining.

X & Z axis of the slide are less than 0.005mm.4 jaw chuck has been using for both the operations.

Speed in the second operation, is min.500rpm to max.1000rpm and feed is 0.08mm/revolution.

In the second operation, the 82.5 dia has been clamped & first side facing has been rested.

I had to translate that into English measurment so that my limited mind can relate. You have a roughly 4" x 5.5" rectangular plate that you are holding on either a face plate or a 4 jaw chuck. You are facing the plate and turning a 82.5mm dia boss X 5mm long. Then you flip it over and hold it in a 3 jaw chuck? Special collet? Fixture? .02mm translates out to less than .0008 thousandths in English measurments. That is a pretty tight flatness tolerence to expect from that setup. If you have bored and faced chuck jaws to hold the second operation have you undercut the jaws to make sure a sharpcorner of the part is not keeping it from fittng flat into the jaws? Can you leave .1mm to .2mm on the surfaces and finish the part on a surfsce grinder.

4 jaw chuck has been used for both the operations. In the First operation, Hard jaws were used. In the second operation, soft jaws were used.

During second operation, a round piece was hold in the center for boring & facing of jaws. A chamfer has been made in the jaws entry so that while clamping 82.5mm dia the workpiece fitted flat on the jaws.

Surface grinding will be uncomfortable as see the drawing.

Also Speed in the First & second operation, is min.500rpm to max.1000rpm and feed 0.08mm/revolution.

During facing operation(second operation), i also found that parallelism towards the center reduces from 0.04 to 0.00mm while dialing circularly.

Dear Umamakeshwarn,

I am unable to down load the drg due to some problem . Please Fax the Drg at + 91 2692 236577 or +91 2692 235332 to enable me to study before I give any comment / solution.

In any case tolerance for Prallality of 0.02 mm for the size of job indicated is reasonably close for Facing operation on Lathe either Normal or CNC controlled. For such accuracy machine tool should have good geometrical accuracy and alignment of Axis and must be orthogonally right. What is the make and Model of CNC Lathe deployed and when was it installed ? The rading of 0.005 mm are as per the test chart given by the supplers or have you checked and verified ? If so how ? I have come across many situations when errors are more in squareness. It may also be possible that Axis of Spindle may not be parrallel to Longitudinal traverse and cross traverse may be at an angle to the axis of the spindle rather than 90 degree. These are very critical test that determines the performance of machine tools and user segment many times ignores the importance on grouse of time. More often than less chasing a few microns is like chassinga wild goose. I am not suggesting this is the sitauation at your end but this is just a feed back based on my experiance and it is always god to check every loose end prior to reaching a final result which I have no doubt -- VERY IMPORATANT FOR YOU

Ideally for this kind of parts to have good flatness within 0.02 mm parts must be Lapped on Lapping Mchine

By the way how was flatness checked ? Many a times people confuse flatness with Parallality and check flatness by using Dial Gauge Stand after placing the job on Surface Plate. In such set up what you check is Parallality and not the flatness ,however for checking parallality parameters it may be alright but extreme care is required to ensure that parts do not have burr and surface plate is cleaned well and there is no dust / inclusion of foreign particle between the Part and surface plate. For flatness of such small job it would be appropriate to use Flatness checking Gauge which our company Micro-Flat is offering and details may be sent in case you inform your address.

Also for checking orthogonality of X & Y axis it is abolutely necessary that right kind of qualified artifacts are used such as typically used by Machine Tool builders and refurbushers. We also offer these to many Machine Tool builders like HMT / LMW / Parishudh / Lokesh Machine tools / BFW / Mazak ( Service Centeres in India ) / Jyoti Automation / Batliboi.

It is also advisable to peridically check the machine for diagonstic test using Ball Bar which would give many type of information to take the decison for reconditioning if required.

In my opinion Lapping Operation would be the most ideal solution which incedently is not very costly and you may consider if volumes permit Please fax the drawing. Thanks

Udayan Patel

does the low and high spots of paralelism error occur in the same places relative to where the part is chucked? seems like you could do a lot more investigation (design of experiments)

Hii

I never thought that thread would gradually arouse interest to this level. It is for this reason I like such activity that forces you to probe more even for simple problems ( Seemengly Simple )

Well the high and low spots during parallality check woulkd remain at the same place regardless of spots for check. For manufacturing metrology normally you scan the surface by moving the stylus of Dial Gauge over the surface as much as possible . If by any chance Highest spot or lowest spot escape the scan it does not reflect in observation sheet

Even while checking on 3 D CMM it may get un noticed as operator would like to ensure that through put time is min possible and 3 D CMM uses sooftware which are based on alogorithams and generally uses best Fit while reporting the value.

These days high end of the machines ( 3 D CMM - CNC Vesrsion ) uses continous scanning Probe like REVO recently intoduced by Renishaw - UK which I saw in one of the exhibition in India. This probably would cover much larger area under the probe at a highly rapid rate and reduced through put time -- bu at what cost ? These REVO is truely revoluationary but highly costly.

For all practical purpose in manufacturing Metrolgy finding the heigest / lowest spot is not the objective as major consideration is exactness for assembly .

Udayan

The right tool for the right job....

Most CNC lathes will have a difficult time holding the tolerances you are expecting from it. Anything below +/- .0005" is considered "high precision" and are usually in the the realm of precision grinders. Why can't a CNC lathe or mill produce results with such low tolerances? Because the action of the tooling and the clamping system and the need for the ways to slide require a small amount of "slop" even if there is a preload on the bearings. Cumulative "slop" between spindle bearings, X axis slide ways Y axis slide ways can account for a good deal of slop. Add tool wear and the forces that act upon the metal parts of the machine that can cause them to slightly bend under load because of the leverage of a arm from center of force. This isn't taking in to account backlash from ballscrews (unless there are separate encoders that are not attached to the ballscrew shaft) torque, and most important: The cleanliness of the area of the chuck the part sits on. There are a myriad of things that can stick to the chuck that don't compress and that are less than .0008" which will affect the total out come but mostly parallelism. Then dont forget heat buildup. This from a forceful cutting action which takes "pushing" power to accomplish.

Grinding requires much less "pushing" force to accomplish it's purpose, as the idea isn't to remove material to shape, but to remove material to predetermined amount to within tight tolerances (of error) of thickness or diameter.

When you get down to machining at these low tolerances, the amount of causes of error increases. Even the machine level is critical. Many times machine brochures will advertise the ability to machine to tight tolerances, but remember, this is a "best case" scenario and is used more to sell a machine than to operate it.

It would be better to rough the part and precision grind the part afterward with a CNC 2 or 3 axis grinder. These operate in tolerance range of around .00005".

You may be pushing your lathe to the edge of it's ability. It will only get worse as the machine gets older. Consistent good results from a skilled machinists comes from using the right tool for the job. Some may occasionally get acceptable (below .0005") parts from a machine such as this one. But if you ever did get such parts on a long run with tolerances higher than .0008", then it is your setup that is bad now; wrong tooling choice, feeds too fast, or spindle too slow, clamping pressure too high or too low, poor material (casting cooled too fast on one side, do hardness test to see). Each machine has a limit to it's precision machining capability. So does a machinist. Finding the problem in a lack of precision results from a machining operation starts with enumerating all of the possible causes, and eliminating them one by one. Unfortunately you have to do it yourself, we can only offer ideas as to what items to put on the list.

Error stack up is great point.

However, by what means was machine capability initially determined?

As both you and GAryceng above pointed out, machine capability should be determined prior to accepting work. 1) WHat was Cpk for "flatness" on each of these process steps?

2) what was Gage R&R? for the determination?

Process control plan should give you actions to take when system goes out of control, let alone specification. Your Failure Mode effects analysis made prior to starting the job would be the document to check to 'recover.'

milo "It ain't the same quality, if it ain't the same Quality.

The question was intended for the original poster.

If you would like to send that part to North Carolina, USA perhaps we can fix it. I have 40 years of experience. I have not worked in 7 years since most manufacturing has been sent elsewhere because of price. Maybe price is not everything?

Surface grind both sides and you will easily get that

Hi !! Kamesh DVK

I trust after getting inputs from so many contributors you have got the lead to solve your problems/

Good Luck

Udayan

Hi there,

My name is JP Diederiks.

Well I'm not in this game, but do financing of all equipment on a rental agreement where you get ownership after rental period.

There is a person named Koos Snyman that can probibly help. He is in Brits, SA.

Contact number 0824941929

I hope I could have been any help.

Good day,

JP

How much pressure is used to chuck the piece in the first and second operation, it may be distorting at unclamping. As mentioned earlier, are you checking flatness or parallelism? two surfaces could be parallel and not flat, think of a horse shoe. Functionality might be asking for more. A flatness and parallel callout may be needed. Also, if you are using a four jaw chuck on the outside of the square, this can also be causing a problem. If the first surface is not perpendicular enough to the outside square of the casting, than this can throw you out when you face off the opposite side. Since the clamping pressure is against the outside of the casting, this is now your primary alignment, if possible, consider having the clamping pressure against the face, not the outside.

Finally i decided to go by surface grinding after all tryouts....

Thanks for everyone for their ideas....