PDA

View Full Version : Need to make 24 of these



Smokedaddy
12-18-2008, 08:14 PM
Looking for some advise from those in the know. I need to make 24 of these out of 6061. I will cut the 5 inch long 3 inch cylinders on my bandsaw and face them on the lathe. This will be the first time I will make money on anything. Everything else in the past has always been free or for buds of mine. Any machining tips, tooling, machining the pockets, setup, jig etc., help would be greatly apprecaited to cut my time. I have a EMCO Maximat v10 and an old Bridgeport. I don't mind buying tooling if it saves time.

http://www.pbase.com/smokedaddy/image/107221651

Thanks in advance,
-SD:

Mcgyver
12-18-2008, 08:30 PM
how to go about it has everything to do with tolerances. For example off far off concentric can the bores be from the cylinder for example, do the counter bores have to be flat, how concentric do they have to be, how much wander is permissible with hole etc.

I'd consider getting the service centre to chop them to length. they'll have a blade with enough tpi for 3" stock, us home shop guys usually don't. you save time and probably money as their big saw will make very square cuts where as you have a cheapo with high tpi it can wander more easily - that uses more material. that and get a bunch of different quotes, service centre pricing depends on moon phases it seems. they'll budget a 1/8" saw kerf - are you going to be able to hold to that on your saw?

Liger Zero
12-18-2008, 08:34 PM
Whats the part do?

torker
12-18-2008, 08:59 PM
That's very cool! How you gonna weld them little pipes in there?
Sorry..I just had too...

Stepside
12-18-2008, 09:37 PM
I would be concerned with the 3 inch long 1/4 inch bore. Does it have to be concentric to the counter bore on each end? A long 1/4 bit can be pretty flexible. Or even worse are they a reamed hole that is concentric? Is the tolerence indicated by the drawing the desired tolerence?

Smokedaddy
12-18-2008, 10:03 PM
I was asked to make one so they can see if it works, then make the others. The bores need to accept a piece of 1.625" copper tube. A tolerance wasn't given to me, probably 3 thousands? It needs to fit just like a piece of 1.625" copper tube would in a 1.625" copper fitting, like a 90 degree elbow for example. Concentricity isn't that critical, nor is the perpendicular bore. The bottoms need to be flat but the flatness isn't critical either. The .25" bore isn't critical either, it is just for a argon gas purge. I think my bandsaw cuts pretty accurate but I will ask about the cost of pre-cut pieces.

http://www.pbase.com/smokedaddy/image/107223418

Any suggestions are appreciated, tooling, cutting the bores etc.

Regards,
-SD:

mechanicalmagic
12-18-2008, 11:49 PM
SD,
For the cutoffs I would use a 4 tpi skip tooth blade. Pick the shortest one then:

In the lathe: (assuming a QCTP)
Face one end, break edge, 45* angle for chamfer.
With a cheap turret tailstock:
Spot drill
pilot drill 3/16", 1.5" deep
drill 1 1/4" 1" deep from touch
Set saddle stop
Bore to size, one rough cut, two finish cut to size.
with the turret, drill 1/4" to 2.5" depth
Return facing tool, cham bored and drilled holes.
repeat.
THEN do the other ends.

In the mill:
set an end stop on the vise
place first part in mill vise
MAKE SURE boring bar and all tools fit in the vertical space.
find center
Spot drill
1/4" to intersect
1 1/4" to depth
Bore to size.

This is based on my machines, and my style, YMMV.
Dave J.

Smokedaddy
12-19-2008, 12:34 AM
Dave,

Do they make a 1 1/4 bit for a #3 Morse Taper (I think that's what mine is)? I haven't a clue as I've never bought a morse taper bit. Or I assume I would need to buy a bit with a turned down shank. Think my lathe can handle a bit that large? Sure would be nice.

http://www.pbase.com/smokedaddy/image/107227294

http://www.pbase.com/smokedaddy/image/107227292

Oh, and how would I make the bottom of the bore flat (if that's what they want)? It doesn't have to be perfect, just aesthetically pleasing.

-SD:

lenord
12-19-2008, 01:11 AM
SD,

MT for a drill bit, ouch !
I have a 9x20 and used a 1-15/32 bit in some Al. today, not a problem.
The bit had a 1/2" shank on it in a MT2 drill chuck. Just get one close to the size you need, get as much of the hole as you can with the bit, then usea boring bar to flatten it out and get the ID right. Much cheaper than a MT bit IMO.
My metal man has a cnc saw, and could cut your stock to your lengths in a few minutes. Cheaper if you don't have the time to DIY. Expensive if you do have the time. Oh, if you do have it cut somewhere, make CERTAIN you spec enough length for each piece to face the ends to the right length. For example: If you tell them 6- one inch pieces out of a 6" round, Al., they give you just that. When you have to face it on the lathe, you can have from .850-1.003" finished thickness unless you specify.

Make sure to specify if you have them cut it for ya.

If you have a small 4x6 bandsaw, you can order a 6 tpi blade ( or was it 5 tpi) for it for cutting larger diameter Al. rounds. Works like a charm, much faster cutting. ( I got me one of them ! )

FWIW
Lenord

Ian B
12-19-2008, 01:12 AM
For the flat-bottomed hole, can you find a 1 1/4" end mill (or slot drill) on a 3MT? Use it to finish the hole to size and leave a flattish bottom in one pass. End mills are ground with a very slight fishtail, but it doesn't sound as if this would be a problem in this case.

Ian

ckelloug
12-19-2008, 08:01 AM
I don't know your customer but I'd make them tolerance the thing before committing to it or at least sign off on the tolerances you decide you want to hold. . .

The nice thing about doing things for ourselves and buddies is that we know what will work and can relax tolerances as progress on the part dictates.

In the mold I recently made, one of the end plates is short by .120 in the x dimension because that is what it took to clean up some out of square sawing done by the service center.

If this was a paying job, the part would have to be scrapped and I'd be over at Crucible complaining. On the other hand, since it was for me and a one-off I just made sure to chose x so that that side would not be on the bottom which would keep the part from sitting up as needed.

--Cameron

derekm
12-19-2008, 08:34 AM
SD,

MT for a drill bit, ouch !
I have a 9x20 and used a 1-15/32 bit in some Al. today, not a problem.
The bit had a 1/2" shank on it in a MT2 drill chuck. Just get one close to the size you need, get as much of the hole as you can with the bit, then usea boring bar to flatten it out and get the ID right. Much cheaper than a MT bit IMO.
My metal man has a cnc saw, and could cut your stock to your lengths in a few minutes. Cheaper if you don't have the time to DIY. Expensive if you do have the time. Oh, if you do have it cut somewhere, make CERTAIN you spec enough length for each piece to face the ends to the right length. For example: If you tell them 6- one inch pieces out of a 6" round, Al., they give you just that. When you have to face it on the lathe, you can have from .850-1.003" finished thickness unless you specify.

Make sure to specify if you have them cut it for ya.

If you have a small 4x6 bandsaw, you can order a 6 tpi blade ( or was it 5 tpi) for it for cutting larger diameter Al. rounds. Works like a charm, much faster cutting. ( I got me one of them ! )

FWIW
Lenord

MT is normal for accurate drilling and essential for large diameter- most of my 13mm+ is MT and a fair amount of the less than 13mm that I use for close tolerance work. you can get a 1 to 1.5" cheap on Ebay in the UK 10, $15.
I suggest you work up the operations you want to do assess the tolerances you can work to and then give them a marked up drawing with what you want/can to deliver...
e.g. that you only need a flat in the bottom of each bore is 1.2 times or greater than the thickness of the tube and the remainder can be conical. and that the bore 1.6" bore is -0+0.010 and all other dimensions are +/- 0.010.


If the tubes are glued or soldered in this should be fine.
The description of the application seems that close tolerances are not required. Sending a marked up drawing will make that certain.

davidh
12-19-2008, 08:39 AM
my question would be to you guys that know what your doing. . . .
how long would it take to make just one ? ? ?

10 minutes ?

30 minutes ?

after you had the stock sawed and in your hand.

hunting around for the tools after you start is a real pita then finding your drill is dull or whatever. . .

what would be the chance of the small hole being drilled from each end, actually aligning decently if it were done that way ?

for purging a gas, i would think the bottom of the hole would be better it not flat but tapered about the same as the drill point.

humm. anyone ???

Virgil Johnson
12-19-2008, 08:55 AM
If the bottom of the hole has no function I would drill with 1 7/16 dia drill and bore to 1.5 leaving a small flat bottom lip for the pipe to register on. Of course discuss this with the customer beforehand.

A.K. Boomer
12-19-2008, 09:01 AM
After all parts are faced to length I would do all operations by Mill, Using Horizontal/Vert. V-Jaws on my vise I would center drill and drill the two end 1/4" to intersect and then endmill and bore to size, set up stop and repeat for 90 degree intersect for both the 1/4" and then endmill and bore.

winchman
12-19-2008, 10:54 AM
With the set-true chuck dialed in for the diameter of the blanks, I'd think it would be quicker and more accurate to change parts than to change tools while you worked on each one.

After I got each end faced, I'd drill a deep pilot hole to avoid having a long piece of the drill unsupported while drilling at the bottom of the bored recess.

I'd also consider using the 4-jaw on the lathe to hold the pieces for the work on the side. Leave 3 and 4 alone when changing parts.

Roger

rode2rouen
12-19-2008, 12:45 PM
SD,
For the cutoffs I would use a 4 tpi skip tooth blade. Pick the shortest one then:

In the lathe: (assuming a QCTP)
Face one end, break edge, 45* angle for chamfer.
With a cheap turret tailstock:
Spot drill
pilot drill 3/16", 1.5" deep
drill 1 1/4" 1" deep from touch
Set saddle stop
Bore to size, one rough cut, two finish cut to size.
with the turret, drill 1/4" to 2.5" depth
Return facing tool, cham bored and drilled holes.
repeat.
THEN do the other ends.

In the mill:
set an end stop on the vise
place first part in mill vise
MAKE SURE boring bar and all tools fit in the vertical space.
find center
Spot drill
1/4" to intersect
1 1/4" to depth
Bore to size.

This is based on my machines, and my style, YMMV.
Dave J.


Dave's sequence seems to be pretty realistic....we must have similar shop set ups.
The only thing I would add: Have the customer supply a 6" piece of the tubing they are going to use, with one end prepped as it will be used.


Rex

mechanicalmagic
12-19-2008, 01:20 PM
Dave,

Do they make a 1 1/4 bit for a #3 Morse Taper (I think that's what mine is)? I haven't a clue as I've never bought a morse taper bit. Or I assume I would need to buy a bit with a turned down shank. Think my lathe can handle a bit that large? Sure would be nice.

Oh, and how would I make the bottom of the bore flat (if that's what they want)? It doesn't have to be perfect, just aesthetically pleasing.

-SD:

SD,
Yes, ENCO has them for ~$125 each. Or you can get a reduced shank (Silver & Demming style) for $25, with a 1/2" shank.

For the boring bar: in aluminum, you should have a high rake, given your small machine. I would consider using the largest scrap end mill you can fit into your tool holder. Grind off one flute tip, so it won't touch the bottom. Sharpen the end of the other flute, add a small radius. Set it with a few degrees clearance so the side of the flute doesn't rub.

If you don't have a QCTP: then you can face with the boring bar, turning in reverse. You will need to grind a 45* for chamfer on the far flute.

You still haven't provided any tolerances, do not quote this without knowing that you have the measuring tools and STANDARDS that you trust. For example; it would be common to tight dimension between the flats of the end bores. Not an easy measure without the proper tooling.

Dave J.

Smokedaddy
12-19-2008, 02:45 PM
Me again,

This is for a school that I teach at. Since I am an aspiring machinist <smile> they are throwing some work my way. The only tolerance that would be important is the bore. I have to be able to slip a piece of copper tube in the bore and the fit should similar as if it were a copper tee. The bore debth is the same as a copper tee. As I mentioned in a previous message, I would guess 2 to 3 thousands clearance.

All they want is for me to make them an aluminum tee, that somewhat mimics a 1 5/8" copper tee. The drawing was my suggestion. I figured buying round stock was the least expensive way of doing this and I thought my design was straight forward. This is for a test bench setup used for brazing certification. The brazer sets up on their individual test bench with a coupon, then brazes the coupon with a argon purge. At the moment they use a copper tee setup that you see in the link below. The problem is, the copper tees need to be replaced often as they get destroyed by the students and they are super expensive to replace. Making a aluminum one was my suggestion to the problem.

http://www.pbase.com/smokedaddy/image/107239855

-SD:

Lu47Dan
12-19-2008, 03:48 PM
Not to seem like an A-hole , but ever hear of masking tape ? I am a certified Medical Gas Brazer , and I have tested out numerous times over the years since getting certified . Cap with hole offset to allow air to be purged on one end , hose taped in the other end with the masking tape to hold the hose and seal that end . Braze the joint and do your prep , paperwork and send it in for testing . Masking tape is cheap and plentiful .:rolleyes: Dan

Smokedaddy
12-19-2008, 05:56 PM
Dan,

Don't think you are sounding like an A-Hole, just don't think you know their procedure, or setup or protocol. Masking tape would stay on the 6 inch long 2 inch copper coupon for about 30 seconds. I will take a pic next time I am there.

-SD:

kvom
12-19-2008, 09:36 PM
Seems to me it could be shorter than 5". Total length needed to clear the 3 bores is 3.63, so a 4" length should still work and make the drilling a bit easier.

Seems as if 2.5" dia stock would work too.

gunbuilder
12-19-2008, 11:15 PM
...This will be the first time I will make money on anything. ...:
That is what I hope for on every job.

Have a good holiday,
Paul

Smokedaddy
12-20-2008, 12:10 AM
Seems to me it could be shorter than 5". Total length needed to clear the 3 bores is 3.63, so a 4" length should still work and make the drilling a bit easier.

Seems as if 2.5" dia stock would work too.

Actually they emaild me today asking if I could make the bores a 1/2" deeper. <grin>

-SD:

Lu47Dan
12-20-2008, 02:11 AM
Dan,

Don't think you are sounding like an A-Hole, just don't think you know their procedure, or setup or protocol. Masking tape would stay on the 6 inch long 2 inch copper coupon for about 30 seconds. I will take a pic next time I am there.

-SD:
Our protocol is NFPS for Med Gas Brazing . We use masking tape for ours and it is held at 3G in a welding fixture , so the welding fixture might help dissipate the heat . Granted we use longer copper tubing then you do when brazing the coupling and the two pieces of tubing together . Do you send in the whole pipe or do you just send in a strip for testing ? Dan

Smokedaddy
12-20-2008, 03:27 AM
Dan,

Our instructions are also ATR's, for brazing, but we do send out all of the welding process to a lab for xray. Our copper certification require 100% penetration , no void pockets etc., horiz/vert, will post some pictures in the near future. Anyway, this is the best picture I have of our brazing and soldering lab. We have 24 booths. You can see the aluminum adapter below the copper tee and copper tube, on the side of the table. Stainless steel tube (actually we used ultra high purity SS tube since it was donated) is ran to the back of that aluminum adapter for the argon purge, so there are no hoses to mess with. Some day I will personally take some better pictures.

http://www.pbase.com/smokedaddy/image/107257613

http://www.pbase.com/smokedaddy/image/107257861

-SD:

winchman
12-20-2008, 09:11 AM
Is the thick aluminum section going to soak up enough heat to make brazing the test piece difficult?

Roger

Smokedaddy
12-20-2008, 01:02 PM
Hi Roger,

We've been using this setup for about 2 years now, no problems so far.

-SD:

gellfex
12-20-2008, 02:38 PM
To weigh in on the cutoff issue, I've used a 12" miter saw with 80 carbide teeth to cut off heavy 6061 for decades. a little cutting wax helps. It's much faster and more accurate than a horizontal bandsaw.

Smokedaddy
12-20-2008, 11:50 PM
Just for information ...

I was quoted $11.00 each today for 24 pre-cut (3" dia. x 5 1/8" long) 6061.

-SD:

Smokedaddy
12-21-2008, 11:50 PM
Can anyone in the "know" tell me what a fair price would be for each one of these?

-SD:

lenord
12-22-2008, 12:03 AM
SD,

2.5 times the cost of the material cost is typical. That is the material cost the customer would pay for material, not what you get it for.

Lenord

Smokedaddy
12-22-2008, 01:21 AM
lenord,

Thanks for the input. Guess I was trying to figure out what a real machinist would charge, labor etc., for making one of these. Not per hour shop rate but the total cost to make one of these, or 12 of them. Guess I'll have to take the drawing to a machine shop and get a quote. Thought maybe someone would chime in here that would actually know.

-SD:

lenord
12-22-2008, 01:42 AM
SD,

You are a "real" machinist, as am I.

I do this for money. Now, you do too.

The way it works is, you charge whatever you can get away with. No, seriously, some guys do that. Charge what the market will bear is the mantra I have heard. I usually break down the prices for customers that want it, but as a "rule of thumb", 2-2.5 times the material cost is what I end up charging. Dunno why, it just works out that way.

I usually use onlinemetals if the customer asks for a break down... I don't pay that, but I'll quote that.

My biggest problem when quoting things was thinking I was faster at certain things than I really was.

There was an online place that will get you quotes for a job you specify, you might have better luck there. I forget the name of it though.

FWIW
Lenord

A.K. Boomer
12-22-2008, 09:44 AM
SD,

2.5 times the cost of the material cost is typical. That is the material cost the customer would pay for material, not what you get it for.

Lenord



I think thats the vaguest description Iv ever heard on this site, He asked how much to charge for the pieces, Do you mean jack the material up to 2 to 2.5 times the cost of what you get it for then add what it took to build the part? If so then you forgot to tell him how much to add for that particular part, If not then your statement was for the entire Job, material and labor, that would be a real hat trick since some jobs require 10 or 100 times the labor of what the materials worth and others are only 1/10 the labor of what the materials worth:confused:

torker
12-22-2008, 10:16 AM
SD..I can't tell you how much to charge for those...I can only tell you how I charge for stuff like that.
You are in much the same boat as me.
I am only a wanna be machinist.
Things that I'm not sure about or don't "really" know how to do yet...
There is no way I can charge my customer for my "learning" time.
What I do with something like that...do one...sometimes two until things start to go quick and smooth...then I record the amount of time it took to do one of those and charge my hourly rate for the whole batch. I even do that with the welding end of my business.
I don't care who you are or how much you know...there is ALWAYS something coming in the door that will baffle you...there are ALWAYS screw ups with equipment etc.
I've seen some of the best in the business get bitten on quotes etc. Seen $50,000 losses on screwed up quotes. My "system" works for me and is fair to the customer.
Of course...we always learn ways of doing the same...or similar jobs faster the more we do them. THAT'S where we start making some serious money.
Russ

Smokedaddy
12-30-2008, 10:35 PM
Just a follow up,

I made a prototype today. I will let them use it for a while to see if any modifications are needed. I did most of the work on my Bridgeport and a rotary table. I snuck up on the final I.D. with a long endmill with super light cuts. The copper tube fits perfect.

Question, if I used drill bits to sneek up on the bore I.D., what step increments would be a good idea on my EMCO v10 -or- my old Bridgeport. My equipment didn't like going from 1 inch to 1 1/4 inches. Would 1/8 inch steps do the trick?

http://www.pbase.com/smokedaddy/image/107611415

http://www.pbase.com/smokedaddy/image/107611417

Regards,
-SD:

Fasttrack
12-31-2008, 12:18 AM
Actually, sometimes taking smaller steps will bog down the machine worse than larger steps. The drill bit "grabs" more. Steps work well when you don't have enough down force to get a big bit to bite (like hand drills or etc) but if you've got the down force (rack and pinion quill), steps may only cause your motor to bog down. They make special hole enlarging drill bits that would do the trick nicely or you can regrind the rake on your drill bit to keep it from biting too much. (I'm the wrong guy to tell you about that, though, since I've never done it)

Not sure exactly what kind of problems your having... this may not be the issue.

mochinist
12-31-2008, 12:24 AM
lenord,

Thanks for the input. Guess I was trying to figure out what a real machinist would charge, labor etc., for making one of these. Not per hour shop rate but the total cost to make one of these, or 12 of them. Guess I'll have to take the drawing to a machine shop and get a quote. Thought maybe someone would chime in here that would actually know.

-SD:Dont take this the wrong way but you trying to figure out what a real machinist would charge is basically asking for a quote, and quotes take time and it isn't easy. You could take it to a shop and have them quote it I guess, if you don't mind knowing you are wasting some guys time to quote your part that you're gonna make.

Basically what I am saying is do it yourself:p try and visualize how long it will take you, decide a shop rate($20or$30 an hour for a homeshop???)and then try and make the parts in that time, great if you do, and if you don't learn from it, everyone that quotes any type of job has had too.


Someone above said 2.5times the material cost and honestly that looks like a fair price for that part as long as there is no tight dimensions.
Materials:$11+20%=$11.22*24=$269.28
materials*2.5=$673.2
$673.2/24=28.05

So think you can do it?:D

Circlip
12-31-2008, 11:19 AM
And don't fall into the trap of under estimating the material you need. For the component in the first drawing, you need a minimum of 12ft for 24 components. As for "Sneaking up" on the bore, I would pilot drill and bung as large a hole as you can put through, you can slow the speed down not to have the machine labouring.

Regards Ian

Smokedaddy
12-31-2008, 11:38 AM
As for "Sneaking up" on the bore, I would pilot drill and bung as large a hole as you can put through, you can slow the speed down not to have the machine labouring.
Regards Ian

Don't understand the statement above.

-SD:

Smokedaddy
12-31-2008, 11:45 AM
As far as the larger drill bits go, it seems once I get past the beveled end of the bit it cuts fine, otherwise it just wants to grab. If I take super light cuts then it chatters. The 1 inch and 1 1/4 inch are new bits. I have a super ridgid setup. The RPM was about 1000. Would 1/8 steps solve this problem. If so, I am willing to buy a couple of more bits.

-SD:

Mcgyver
12-31-2008, 01:37 PM
The 1 inch and 1 1/4 inch are new bits. I have a super ridgid setup. The RPM was about 1000
-SD:


\:eek:

i forget what the material is but that is way too fast imo even if its aluminum. forget theoretical maximums, on big drills, slow it way down. I'd start at 100 rpm, with a less-than-1/2" pilot. you'll have more torque so will be able to feed faster, partially making up for the slow speed.

Circlip
12-31-2008, 02:10 PM
Put a clearance hole through first and use the largest drill you can at one go. Don't step drill, so you're only taking a finishing cut with a boring tool. Like everything else, machining is an aquired art and although the reference books give the theoretical feeds and speeds for cutting various materials "Feel" comes into the equasion in HSM and the more you do with differing materials the better the feel gets. You can tell very quickly if the machine is labouring.

Regards Ian.

Fasttrack
12-31-2008, 02:33 PM
Yep - I was always taught that you can't drill a decently round hole by stepping up bit sizes like that because of the chatter. (Granted this was in regards to using a drill-press) It tends to cut almost a triangle for the first little bit. Like I say, some here could probably tell you the proper way to grind a drill bit to keep it from doing that or you can buy bits specifically designed for enlarging pre-made holes.

Otherwise cut it in one go with the largest possible bit and then use a boring bar to finish it up. Or you might get away with a drill bit if the material to be removed is very tiny.

Smokedaddy
12-31-2008, 05:42 PM
Damn,

I just went with the speed and feet calculator which calculated it at;

Cutting speed (FPM): 350
Drill or reamer diameter (inches): 1.25
Revolutions per minute: 1070

Thanks,
-SD:

mochinist
12-31-2008, 06:43 PM
100rpm is way too slow, he's trying to make money now:), 1000rpm would work fine(in aluminum) but you have to have a good feed, if you baby it, it's going to chatter, try like 500 to 600 rpm and ditch all the step drilling, you just need to pilot drill a hole bigger than the web on the final drill.

lane
12-31-2008, 07:52 PM
1 1/4 drill how about trying 50 -75 RPM with a 1/4 are 3/8 pilot hole I wish you would throw them speed charts away . Every thing you try to do you running way to fast about 10 times to fast. Those charts are for a cnc lathe running cub drills. You got a little bity lathe. I told you that 2 weeks ago.

Smokedaddy
12-31-2008, 09:48 PM
Hi Lane,

I got the RPMs from the Little Maching Shop ...

http://littlemachineshop.com/Reference/CuttingSpeeds.php

... also, even though I was wrong with the speed, the 1000 RMP was on my Bridgeport.

Happy New Year (almost),
-SD:

Smokedaddy
01-10-2009, 01:06 AM
Just an update,

Amazing what slowing the speed down and increasing feed did. I was amazed how it cut like butter, especially on my old Bridgeport. Thanks for the tips.

-SD:

Circlip
01-10-2009, 07:39 AM
Nice feedback SD, just like the driving test, you get a piece of paper to tell you that you're competant to drive a vehicle on the public highway, THEN you learn how to drive.

Regards Ian.