citizen sliding head lathe

"ppm" wrote in news:1152074995.559456.251440 @v61g2000cwv.googlegroups.com:

===================== @684$US that's a spicy meatball!!!!

except for the price I would like to have one for my small lathe.

Is all swiss tooling this expensive or just SPI?

Try google look for Zeus knurling tools.

Contact Alouette Tool Co. in Fairport NY. and talk to them about Efanger knurling tools. Look to be the same thing as mentioned below but they aren't nearly as expensive. We use them on all of our Star Swiss type lathes.

585-388-1240

D Murphy wrote:

F. George McDuffee wrote in news: snipped-for-privacy@4ax.com:

The problem is finding something that will fit into the small tool zone of that machine.

As it is the tool I linked to will likely take up two positions. The B12 doesn't have too many positions to start with. Without seeing the part or getting a better description it's hard to say if something less expensive will do the trick or not.

He may be able to bump knurl it with a cheapo holder.

Try these guys

carry cut knurling tools, which involve a lot less tool pressure but are dicey to use if you are going up to a shoulder. But in that case they have standard also, & there stuff is not as pricey as that of many others such as Zeus. Call them up and explain what you are trying to do, they will help you.

-plh

Dear all, when drilling diameters in the range of 1 mm to 6 mm which type of er collets are better? ER9 OR ER11 ? PPM

"ppm" wrote in news:1153282626.314556.186400 @s13g2000cwa.googlegroups.com:

Not much difference really. In the US ER9 collets are relatively rare. ER8's are more common. I've used both the ER11 and ER8's for small hole drilling with good results. If you were drilling smaller than .5mm, I would go with the ER8's or 9's for a straight shank drill.

The important thing is to buy the collets in .5mm increments rather than the usual 1mm. Buy high quality extra precision ones, either Swiss or Japanese made if possible.

Never go over the collet capacity. If you have a 2.1mm drill, it's better to use the 2.5mm collet rather than the 2mm. It may seem that the

2mm is a better fit, but trust me it's not. The absolute best situation is to buy the collets to match the drill shank. For small holes (less than 3mm) I like to use drills that have a larger common size shank. There is more surface to grip on and you are not squeezing the collet down at all. A 1.3mm drill with a 2 or 3mm shank will line up better than astraight shank drill will, being held in a 1.5mm or worse yet a 2mm collet.

If you are drilling these small holes on a Swiss type, and if your machine is capable of superimposed machining, you will get the best results drilling small holes by parking the Z1 axis in the + direction, by at least the hole depth distance, and drilling into the end of the stock with the Z2 axis.

In any case buy high quality collet chucks and collets. And be sure to check the alignment of the drill to the spindle with a dial test indicator. You should be under .0001" (3 microns) TIR.

Good luck.

Dear All, A. Chip problem in SS:

We are presently doing job which is 8 mm in diameter and 9mm overall length. The material of the job is SS304. The component has 2.35 mm dia through hole and another 3.5mm dia hole for about 5mm. there is an step turning in the OD. When we do this in our citizen A16 machine there is lot of chips( spiraling) coming . Esp. in the drilling because of which we are removing the chips for every component machining. This is taking our machine time. Is there any suggestion to avoid this problem.

B. Threading:

For another job, which is of carbon steel, we are having a thread spec of 3/8-16 UNC. For which we are using G32 (repeating for 11times). Is using G32 or G92 better than this?

Is it possible to make worm gear cutting in B12/A12 citizen machines?

===================== Because pi [3.1416] is involved, you wind up with either weird TPI/pitch numbers or weird PD/module specs when making worms and worm gears.

CNC is uniquely suited for this, although cutting worms to function with standard PD/modules is frequently a problem with the older mechanical systems that relied on gears and lead screws, and in fact is impossible to do exactly, although millions of worms that were "good enough" have been machined.

Effectively you will be cutting coarse/quick Acme [29 degree inch] or trapezoidal [30 degree metric] thread relative to the diameter. Given the amount of material that will have to be removed it is likely you will have to use live tooling to mill the thread. Tooling will likely be expensive [but then what tooling other than standard drills is not expensive on a "Swiss.?"] and set-up [helix angle] may be "delicate." Although it may be possible to "single point" small worms, Acme/trapizoidaly threading tools in the small sizes required may not be a stock item.

The more useful question to ask may be to ask "can I make small worms on my A16 that I can sell in my market for a profit at the same price as worms made on other machines or by other processes?

This will depend your market and customers. You may also want to consider using stock with the worm thread roll formed.

Unka George (George McDuffee)

...and at the end of the fight is a tombstone white with the name of the late deceased, and the epitaph drear: ?A Fool lies here, who tried to hustle the East.?

Rudyard Kipling The Naulahka, ch. 5, heading (1892).

"ppm" wrote in news:1154062307.091707.262560 @h48g2000cwc.googlegroups.com:

Use the G83 peck drilling cycle. Remember to set the PECKC parameter.

G83 Z#.## R1.0 Q2350 F0.06

Too many passes for starters. There's no real difference between G32 as far as the cutting path goes. G76 allows angular infeed and might do a better job.

Remember when you use G32 or G92 to calculate the depth of each pass so that you are removing a constant volume of material, rather than a constant depth of cut which takes an increasingly larger volume with each pass.

"ppm" wrote in news:1154062437.553125.36250 @m73g2000cwd.googlegroups.com:

You should be able to cut it using a threading cycle. If the machine is accurate enough (should be) and if it's rigid enough (could be a problem).

============ I am not a cnc or swiss "expert" but 11 passes seem excessive, particurarly for carbon steel. Is there anything special about this steel? Hardness? Machinability? What thread tools are you using? What rpm? Are you machining to a shoulder? Are you allowed a thread relief? Does the end require special finishing? Higby thread? Are you more concerned with tool life or production rate?

Given the age of your machine [new] and assuming "normal" MS steel & part configuration, I *GUESS* you should be doing this in three passes, possibly with one additional very light finishing pass at higher speed for primo appearing [polished] threads.

G32[block]/G92 is the "traditional" threading command and on most controls [I am unsure about the Oi-TmodB] this advances the tool straight [radially] into the part for each pass. The difficulty is that the tool cuts on both sides of the V, with operationally negative rake on the trailing flank. The chips get wider as the tool cuts deeper, and tend to jam where they meet. Because the chip *RAPIDLY get wider as you go deeper, you need to progressively reduce the depth of cut to avoid chatter and other problems.

The alternative is the G76 command which advances the tool at an angle [2 axis move] into the part, generally slightly less than the included angle of the thread. Almost all cutting is done on the leading edge of the tool with only a "burnishing" action from the trailing edge. This cuts the chip width in half, and the leading face operationally has a slight positive rake. You will need to set the A parameter for the thread form.

Many toolmakers and better machinists on manual lathes will use the compound [top slide] to advance the tool at an angle for all the passes except for the last light finishing pass where they advance the tool radially. This was susposed to give a better thread and eliminate any visible "steps." although an advance angle of slightly less than 1/2 the included thread angle burnishes these out anyhow.

Anyone out there that is using G76 for rapid removal and a G32/G92 for the last pass?

For a more complete discussion see p339-356 Smid, Peter "A Comprehensive Guide to Practical CNC Programming --- CNC Programming Handbook" Industrial Press :NYNY ISBN 0-8311-3158-6

I have the 2nd edition, and a later one may be available.

See:

?z=y&btob=Y&pwb=1&ean=9780831131586 There are many other books available. See google for titles/sources.

I notice that the technical schools in India are greatly increasing the amount of CNC materials they are covering. Try contacting your nearer technical schools and engineering universities. These are generally goldmines of information and you may be able to recruit an intern or work-study student taking upper level cnc courses.

Unka George (George McDuffee)

...and at the end of the fight is a tombstone white with the name of the late deceased, and the epitaph drear: ?A Fool lies here, who tried to hustle the East.?

Rudyard Kipling The Naulahka, ch. 5, heading (1892).

========================== There may be some language problem here. In the following discussion I am assuming: bib = cut-off pip or tit work piece seperator = cut-off [parting] tool.

This can be a problem and indeed some of the older screwmachines had a special attachment to remove the cut-off pip.

While it will involve additional cycle time and tools, you can eliminate [or at least minimize] the "bib" by grinding the cut-off tool at an angle. This will more-or-less eliminate the cut-off tit on one side while making it worse on the other. This is generally done so that the tit is on the bar stock in the machine. The extra cycle time comes in when you face off the tit on the bar stock before starting to make the next part. You don't need a open side working station as you can use something like a center drill or center cutting endmill in an end working station.

And there is always the traditional method of careful application of a fine file, possibly with some sort of guide or fixture to eliminate "over burring."

Unka George (George McDuffee)

...and at the end of the fight is a tombstone white with the name of the late deceased, and the epitaph drear: ?A Fool lies here, who tried to hustle the East.?

Rudyard Kipling The Naulahka, ch. 5, heading (1892).

"ppm" wrote in news:1155728415.447650.14750@

74g2000cwt.googlegroups.com:

Well you could just use the sub spindle to eliminate the cut off tit. You can also grind an angle on your tool 10-15 degrees across the face so that the work seperates from the bar first. It also helps to cut to a small diameter say 1.5mm, then drop the rpm and the feed rate, and feed the rest of the way to part off.

If the problem is that you don't have the proper subspindle collet, but you do have a larger one, you can also make a work support bushing and mount it in the sub spindle or even a drilling station. The work support bushing should have a bore slightly larger than the work O.D. and should be milled in half for a distance at least equal to the work length at the support end. Then just bring it in to support the work during the part-off operation.