Fluted Posts

[cbradshaw]

I have some post that I need to flute and I want them to taper or pull up at the ends. Can someone tell me how to do this?

Thanks,

Carroll

[srwtlc]

Carroll,

What cam software are you using? Are you saying that you want to use a round nose bit and pull the bit up gradually to bring the flute to a point (sort of)? You could manually program it by determining at what point you want to start coming up and do a M3 to the end taking the Z up to zero or if your software will allow it, you could draw a arc in the Z axis and break it down to a bunch of small M3's.

[Brady Watson]

Carroll,
You could set up the post on the machine and plunge the bit to the depth you want on the 'fat' flute end of the material...we'll say MZ,-0.5 for example, and the post is 48" long...Tell the machine to do a: M3,48,Y,-0.25 where Y = your Y position. This will gradually pull the Z up from your starting point in X to 48" lifting the bit a little as it approaches 48" on the X. So if you start the bit .5" deep, in this case it will pull the Z up to a height of -.25" when it gets to 48" on the X.

Does this make sense?
-Brady

[rexhalt@montrose.net]

If you use a 1/2" diameter Ballmill cutter, the ends of your flutes will be tapered, or rounded at the ends, just by pulling straight out of the cut. Try it and see if that is what you are after.

[waynelocke]

Carroll,
I have used vector and drawn a z sloping line at the beginning and end of the flutes. Brady's programming solution seems straight forward and easy. I plan to steal it next time I do flutes.

A tapered pullout is a much more refined ending/beginning than a simple pullup and comes to a curving point. Also, a straight pullup seems to have more of a tendency to burn sometimes. I have always heard these referred to as fingernails and without a cnc they have to be carved by hand. For me, it is a real value added touch that the cnc allows.
Wayne

[Brady Watson]

If you want to do a more 'acute' pull-out at the end, then just do something like this:

(This example not doing long X-move taper)

Save this code to a new SBP file and run in Preview mode to see how the tool moves:

MZ,-.5
MX,47
M3,48,0,0
JZ,1

-Brady

[garyb]

Carroll, I draw the flutes in cadd then use the center line "V-Carve" and use a bowl or ball cutter, it makes it easier to use the same cutter for different width flutes and it will automatically take care of the tappered pull out that you are looking for.

[bleeth]

Carroll-If you have the latest Windows version of the SB software (SB3) go to tools and check out the Forney fluter. Using a v bit it will pull up and taper perfectly. It does, however, make all the flutes the same width and sometimes I like my center flute longer.

Dave

[cbradshaw]

Thanks to everyone that replied. I didn't know there was a Forney fluter. I'll probably try all our your recommendations.

This forum is the best.

Carroll

[jkforney]

Not only is there a Forney fluter, there is a Forney

[bill.young]

Hey guys,

No promises but I'll add tapered lead-ins and lead-out to the Forney Fluter wish list. I have a question, though, for the "fluters" in the crowd.

Should the tapered sections be straight-sided like you would get from an M3 move going up to the surface? Look at the top picture below...there's a small radius at the start of the taper but it's awfully small.

Or should the taper have curved sides like the bottom picture by doing a curve with the z-axis as the taper is cut? The straight taper would be easier to add to the Fluter but the curved one looks nicer to me.


4808

What's the preference?
Bill

[hespj]

The curved one looks nicer and is surely quite simple:


4809


4810

A straight ramp upwards gives a curved end.

[harold_weber]

Hey Bill,

Now I know I ask you to add gradual pullout to the ends of the flutes last year.....

Now that you are asking for a preference of what kind of pullout - I prefer to have the runtime option of doing either!!

The shops around here don't use a VEE bit, they use a corebox bit. The attached photo shows that they don't get multiple flutes very consistent (they don't have a ShopBOT).

4811

[bill.young]

Hey John,

You're right, a round-nose bit does do a nice curve like that but v-bits cut the straight-sided tapers unless you curve the toolpath. The Forney Fluter calculates the flute spacing for whatever bit you want to use and calculates the depth-of-cut for round-nose or v-bits, based on the width of the flute.

Bill

[bill.young]

Hey Harold,

I KNEW someone had asked about that before...

[bill.young]

Does anyone use a v-bit for fluting?

[bleeth]

Sure-all the time-In addition to stop fluting it is a distinct custom difference from mass produced millwork.

[Brady Watson]

Bill,
I use a v-bit for fluting from time to time...a tapered ramp into and out of the material would be helpful. Taking this concept one step further, I would imagine that it would be very appealing to have a canned ramp that could be used for cabinet doors etc, where you do an M2, and then append a ramp move to it to sharpen the corners. Just like the CR command, it could be a canned "4,3,2 or 1" quadrant ramp depending on which corner you wanted to do with a custom cut.

So let's say you wanted a sharpened corner with a 1/2" v-bit. You could tell the 'wizard' that you are using that bit and that the inside corner coordinates are (for let's say 12 X 16" rectangle with 1" border) :

Corner1 = 1,1
Corner2 = 1,15
Corner3 = 11,15
Corner4 = 11,1

The code would (roughly & in theory) look like this:

M2,1,1
MZ, -.25
*Add corner with CustomCut
C10

------C10.sbc------------
M3,(&XVal - .25), (&YVal - .25), 0 'Move out & up
M3,&XVal, &YVal, -.25 [or stored current &Z-val) 'Move back to -.25 depth to prepare for next M2 straight move

'Move to next corner
C20 'sharpens next corner
'Move to next corner
C30 'sharpens next corner
'Move to next corner
C40 'sharpens next corner

Just an idea...the code needs some work for sure.

-Brady

[bill.young]

Hey Brady,

With a little trig you could calculate how to sharpen the corners of any regular polygon or really any polyline path...

Definitely has Virtual Tool potential.

Bill

[richards]

Hi Brady,

Your code shows the basic idea very well; but, as they say, the devil is in the details. None of my 90-degree cutters were truely 90-degrees. In fact, the cutter that I currently use gives really good corners when I punch in the numbers for a 88-1/2-degree cutter. As Bill pointed out, dusting off the old calculator and using a little trig can give amazing results on any polyline path.

[Brady Watson]

Mike...I know whatcha mean. When accurate cuts are required, I buy specific brand tools that I know are dead on the money. For decorative work...I use the cheapies


-Brady