Turning a tapered column

[johnm]

Folks -

I've just set up our lathe similar to Wayne Locke's setup, sans the stepper...

Quick question on a time estimate - I need to run a taper on a column from 3" in diameter to 1" over 36". I've got a spindle and can use any cutter.

For those that've done this, I'm all ears - time estimate, bit & feed/speed suggestions, how not to tear up 1) the spindle, 2) the work and 3) Me...

TIA,

John

[robert_cheal]

I am all ears too, I am about to set something up and just not brave enough to try anything yet.

Robert

[Brady Watson]

Gents,
Go to: C:\Program Files\ShopBot\Virtual Tools\Indexer and read the "Indexer Virtual Tool Instructions.pdf" There are several good tutorials in the PDF. Addtionally, in SB3, go to Tools->Indexer and mess aroud with some of the different options you have. Bill Young did a great job (and Grant too) supplimenting the indexer documentation and created many utilities to make life easier.

If I wanted to create a tapered column, I would create an angled line in PW, Insignia or ArtCAM and use the Indexer utilities to make that profile into a rotary file. You'll get a good idea how to do this by reading the PDF.

As far as feeds and speeds go, you can get a good idea by using a block of insulation foam (white, pink, blue etc). You can glue up blocks using wood glue. Then, just start milling. If you make a mistake, you'll only be gouging foam...not wood. It's a great way to have your 'training wheels on' until you get how the indexer (and generally how CNC) works.

-B

[bill.young]

hey John,

[disclaimer. This is strictly theory..consider it a starting point]

I would first look at the available rpm's of the lathe and how they relate to the REAL cutting speed...how fast the material is moving past the bit. If you multiply the diameter of the blank by PI (3.14159) and then by the revolutions per second (RPS) of the lathe (which is rpm/60), you'll find out how fast the material will be moving past the bit. Think of this as the speed that you would be moving the bit through the material if it was laid flat and you were making a straight cut. Remember that this motion will be perpendicular to the motion of the tool, though, so it's not like you'll be trying to push the ShopBot this fast. It will give you an idea of what the bit's going to have to be cutting, though.

Diameter * PI * RPS = "virtual" cutting speed through material

Try some different lathe speeds until you get something reasonable for that "material speed" value, then you can use that RPS value to calculate the move speed of the ShopBot.

The other value you'll need to decide on is the stepover, the distance that the bit would move down the length of the blank for each revolution of the blank. That would be the amount of material that was constantly being cut off the blank, just as if it was a long straight cut. Don't have a clue what that should be...I guess it depends on the power of your lathe, the kind of bit you're using, the material your cutting, and the depth of cut for each pass, how smooth of a cut you're looking for. Remember that the smaller this number is, the less bite the bit is taking on each revolution. I'd suggest starting small and shallow and increasing as you feel comfortable

Now take the RPS of your lathe that you decided on earlier and multiply it by the stepover value that you want and you should get the speed that the ShopBot should be moving down the blank...the move speed setting for your ShopBot.

(rpm/60) * stepover = ShopBot speed value (MS)

Once again this is all theory but I think it will give an idea what will be happening at different settings...hopefully someone will chime in with some "real" experience. My vote is to start slow and speed up if it seems safe (and don't stand in the line of fire in the beginning!)

Bill

[bill.young]

(Brady's idea about using foam in the beginning is a very good one!)

[waynelocke]

You could use the Indexer tools as Brady suggested. Without the stepper I would assume that the software would run the file and show the B axis turning although nothing would really be happening.

You could also just write a file that would begin, oddly enough, at the beginning and just have a J3 move, such as J3,36,,-1. This would taper the piece from 3" diameter to 1/2" diameter in 36". If you zeroed the Z 1" above the finished diameter, you could begin with a small stepdown in the fillin sheet and adjust the speed with the keyboard to what sounded right as the file ran.

If you are starting with a square, then you are only going to be nipping the corners and will have to watch out and adjust for tearing out large splinters.

You should have all of the practice rounds you need to experiment with on the first piece and then be ready to go on the next ones.

Bill's advice and formulas seem like a good starting point. I would also use no more than a 1/2" bit and maybe 1/4".

Wayne

[waynec]

I have a Legacy Ornamental mill, which uses a router to mill many things including tapered columns. Whether or not there is computer control the problem of feed and cutting depth is the same.

The Legacy tapers columns by slanting the bed that holds the stock. The lathe ends are on a bed that can be slanted. The router cuts at a constant depth while the tilted stock rotates beneath the cutter. The fixed pitch of the drive screw determines the stepover, which is about 1/4" per revolution. If lots of stock needs to be removed, as in short steep tapers, you just make multiple passes, with some passes maybe not removing any at all on one end.

I assume you'd have to rotate a straight toolpath in Artcam, so that the rotated path would create a straight column, leaving the tapering to the slanted bed.

Always a way.

Wayne from White Salmon

[gene]

I too have a legacy and it is so simple to taper a collum . Basically the bed is slanted and the cutter the same one i use to surface my table with rides level and creates the taper. I have done 8" x 6" over 60 " on the mill and used them in a bath remodel job

[myxpykalix]

Wayne and Gene,
I don't recall seeing you on the legacy forum. Do you know about this?:
http://groups.google.com/group/Legacy-Ornamental-Mills
I too have a legacy 900 and my only complaint is bed length. That is why i got an indexer with my shopbot. Do you have any pictures of projects you made with the legacy?

[knedert]

Folks:
Sadly, we have been unable to use the Indexer tool like suggested:
"If I wanted to create a tapered column, I would create an angled line in PW, Insignia or ArtCAM and use the Indexer utilities to make that profile into a rotary file."
Because we don't have the Indexer stepper motor.... the Bot control panel locks up and crashes.... I am trying a work-around.... but would LOVE to have an easy way....
Anybody out there with a lathe and Shopbot - but no Indexer have any suggestions????
Thanks in advance,
Rose

[richards]

Rose,
I'm not quite clear on what is actually happening. If I remember correctly, you have an Alpha which needs feedback and without that feedback from a non-existant motor, the controller locks up. Is that what's happening?

If that's the case, and if you selected the 'A' axis as your indexer motor axis, and if your moves are fairly simple, you could just comment out all of the instructions that moved the 'A' axis - or change them to a comment and then issue a pause command so that you would be prompted to manually index the part.

[knedert]

Mike,
Yes.... without the feedback the controller is locking up.... well said.

We just want to make simple lathe turnings. Nothing fancy - just yet....

I will try the "comment out" technique.
We simply want to use the spindle as a cutter for the lathe we have set up parallel to the x axis.

Any more tips? Anybody?

[bill.young]

Rose,

Wayne Locke has the right idea above if it's a straight taper...at it's simplest you really only need a couple of M3 commands while the lathe was turning. One would position it at the beginning of the taper...

M3,0,,1.5

and then the second would move it "downhill" to the end...

M3,36,,.5

If you need to do it in a couple of passes you could just add a little to the Z-axis values to cut shallower. Your whole file might look something like this...

MZ,3
MX,0
MZ,2.5 'first pass from 5" to 3"
M3,36,,1.5
MZ,3

MX,0
MZ,2 'second pass from 4" to 2"
M3,36,,1
MZ,3

MX,0
MZ,1.5 'final pass from 3" to 1"
M3,36,,.5
MZ,3

You'll have to mess with this to get the exact values that you need but I think this should do what you need

Bill

[bill.young]

Rose,

If you want to do a profile like a vase shape, look in the Extruder download for the "Flipper" utility. It would let you draw the profile in Part Wizard and then "flip" it on edge so that it would be all X and Z moves (or Y and Z if that was the way your indexer is setup).

Then you could run this part file while the lathe was spinning and it would cut the profile in the spinning blank.

Bill

[fleinbach]

Rose,


Here is a new post with videos of setting up a standard lath on the shopbot.

http://www.talkshopbot.com/forum/show.cgi?tpc=312&post=46940#POST46940

[knedert]

Yippee!!!
I'm gonna try these ideas.
I just "knew" there had to be a way...
Thanks guys!
Rose

[knedert]

Okay, Folks...
Reporting back in....
I ran with the "Flipper" utility (since the project called for more than just a simple taper), and in the SB preview and air cuts it looked to work fine. Thanks Bill Young!

My concern is that I would like to be able to program in a step-down or roughing path that would take the chunks of wood off slowly.
We seem to have more time than money (for new bits).
According to the extruder info in Bill's Corner, I am to create a toolpath so that it cuts in ONLY ONE PASS.
So I guess my question is: How do I make stepdowns in the Z axis?

I looked at the code that the Flipper program created, but it does not resemble your example above. It "seems" to be measuring from the core of the wood on the lathe, like the Indexer program does.
I consider myself mathmatically challenged, so any "easy" way would be appreciated, like the Extruder and Flipper programs are.

Thanks in advance.
Rose

[davidallen]

Execute the file multiple times using Z offsets.

decrease the offset each time until you're at 0.

[knedert]

David,
Do you mean that I should use a fill-in sheet to do this somehow?
I am not familiar with this.
The archived posts don't have much....and all my mulling around today hasn't been much better! lol
Any tips would be most appreciated.
Thanks,
Rose

[knedert]

Okay,
After 2 pots of coffee this morning, I think I've got it!
Execute the part file...
in the fill-in sheet:
Offset in 2D
change the Proportion Z to 1.5
run the file
repeat steps, changing the Z setting to .1 less each time.
Stop after running the file at the 1.00 setting, as that is the final file.
-- Looks good in the preview... gonna go make some woodchips!
~Rose~WhoSureThereWillBe"Something"ThatGotMissed.. .

[myxpykalix]

Rose,
Take plenty of pictures and post and write down as much as you can to share so we can learn from you!!

[knedert]

Thanks Jack,
My first thought was:
"Oh great... now I'm a guinea-pig!" lol
We'll have an update our latest adventure:
"How we found our Z-zero on the lathe" posted soon, I'm sure!
till then...
~Rose

[johnm]

Folks -

Okay, well - we've got it, sort of.... We've been comparing our cut file sizes with the actual diameter of the object being turned and have been fine tuning.

Here are pictures of the second attempt at turning - the first was in foam. We do wonder what is causing the fretting and lack of the clean cut right at the shoulder - the slight scalloping you see. We had it also on the round tenon end, but I had sanded that off before I thought to take the picture.

Rose and I think it is something to do with the interaction between the cutter geometry and rotation speed of the lathe. Any ideas on how to prevent this artifact? We are using a straight 3/8" plunge bit, and the scalloping repeats at ~5/16" intervals - I think it has something to do with the plunge part of the bit, since this is the radius of the cutter. Any ideas?

Thanks

Rose and John


4863
4864

[myxpykalix]

That problem has to do with the rotation of the bit in relation to the direction of cut. It's hard to tell the direction you are cutting based on the picture. However try it in the opposite direction from what you have there.
If you look at your piece, the opposite side of the cut is clean while the leading edge is rough.

It seems to me that in the indexer instructions it tells you to center the bit over the workpiece. Now i'm not sure how to do what i'm going to explain on the shopbot but here is what we do when we want to turn something round on the legacy (same principle and setup)

We center the bit (say a 1 1/4" bottom cleaning bit) over the workpiece. Lower the bit till it touches the surface. Raise our "stop" the height of the depth we want to cut to get the piece round.
The machine turns the piece while we plunge down and it cuts, however what we do is back the cutter off from the center by 1/2". If you come into the piece from the side (so to speak) as opposed to straight down you get a better cut. If you come into the cut from the backside your cut will be clean on the leading edge of the cut. If you come in from the front side your cut will be clean on the trailing edge (or vice versa)
Now how you program that into the indexer, I don't know and the more experienced users might explain why we wouldn't want to do that if thats not ok to do. I know it works for us on our Legacy Ornamental mill and its the same basic setup only more manual.

4865

4866

[bill.young]

Hey Rose,

Looks like you're getting awfully close!

If you were just cutting a straight cylinder then a straight bit should work fine, but in general with a profile cut the geometry gets funny with a straight bit because it's cutting with the edge of the bit instead of the center as it moves along the blank. It's also hard to accurately deal with any "hollows" in the profile using a straight, flat bottomed bit.

My vote would be to create a file in Part Wizard using the same method as the Extruder...creating an offset with an endmill tool with the same radius as the ballnose bit that you'll cut with...and then using the Flipper to stand it the file on edge. Then cut it with the same sized ballnose bit. Any sharp inside corners will be radiused, but since they're already on a lathe they'll be easy to clean up by hand with something like a parting tool or sandpaper. Remember that since the center of the toolpath is at the center of the ball of the bit, you'll have to adjust your Z-zero by the radius of the ballnose to get the right cutting height.


Bill

[johnm]

Bill/Jack -

Okay, I understand that moving off of "TDC" would give a smoother cut - the wrinkle then, is that by moving off of TDC, you are altering the geometry and your tool cutting position will now be modified and give you a slightly larger diameter cut, since you are now working on the hypotenuse of a triangle, rather than in the straight line of TDC. Now, you could figure out what the position of the cutter on the angle is vs TDC, but some of this is already giving us a headache....

What do you think?

John

[bill.young]

I'd still suggest trying it with a ballnose bit along the centerline of the blank, though I must admit that my experience is with blanks turning at indexer speed and not at lathe speed. At indexer speed it works very well.

There are a handful of ShopBotters that have a lathe setup like this...maybe one of them will chime in with info that's less theoretical than ours!

Bill

[myxpykalix]

John...Pass the BC powder! I don't how about a hypotenWhateverthingamajiggy but you might get some info to give you a better idea of how to accomplish what you want to do by going here:
http://legacywoodworking.com/techniques.cfm

Now this is based on doing it manually on their machine but you might pick up some nugget that might help you in your situation, if not....
YOU'RE ON YOUR OWN! lol

[rnels]

Rose and John,

Might be a little late but here is a file to try.


36 inch 3 to 1 inch taper .5 ballnose zip
36 inch 3 to 1 inch taper 3 inch round blank .5 ballnose.zip (http://www.talkshopbot.com/forum/messages/29/36_inch_3_to_1_inch_taper_3_inch_round_blank__5_ba llnose-18644.zip) (0.8 k)

Please check it out before running. I was stepping down by .1 inch. You could change the file as you would like.

I am assuming you have a 3 inch already rounded blank. Change the MS, JS to whatever you are comfortable with. Zero x at start of taper. zero y at center of blank. ZZero at top of material.

Randy

[rnels]

Rose and John,

I assumed you have your lathe running with the x axis if this is not correct this file will not work.

Also noticed I went too deep I should only be going 1 inch down not two because we take an inch off of each side as it turns. Here is a new file.


36 inch 3 to 1 inch taper .5 ballnose zip
36 inch 3 to 1 inch taper 3 inch round blank .5 ballnose.zip (http://www.talkshopbot.com/forum/messages/29/36_inch_3_to_1_inch_taper_3_inch_round_blank__5_ba llnose-18648.zip) (0.7 k)

Randy

[rnels]

Rose and John,

I have been working on a program to convert .sbp files to indexer .sbp files. My main focus is converting Y to B. However, if you can post or send me an email with the profile you are looking for I can try it on my program to see if it would convert OK (would just take some minor editing as I did on the previous file). This is a work in progress so no guarantees. I would need to know the blank size too.

Randy