Litho Rough Cut / Final Cut

[TimSchubach]

When carving a litho, I understand that I have to do a rough cut to remove the majority of the material using something like a 1/8" ball nose bit, followed by something like a 1/16" or 0.04" ball nose bit for the final cut ( tutorials are good things! ). Assume that there is a frame around the litho, but the size of the litho is bigger than the touchpad ( Shark HD MAKO ). So how do you use the touchpad to SET XYZ0 when you change bits?

Related, where do I find a ball nose bit that small for the final cut? I'm assuming I could use my engraving bit, essentially a 20 degree V-groove, but that would take quite a bit longer even on a small litho.

Unrelated, if I'm doing a photo carving in wood, what kind of finish do you use to accentuate the light/dark areas? Is it as simple as applying your favorite color stain, letting it dry, and then sanding back a little to lighten the close areas? I don't want to screw up a nice carving by using the wrong finishing process.

Thanks!
Tim

[Ms Wolffie]

You reset the touchpad to an uncut spot on your material.
Cheers
Wolffie

[sailfl]

You do not have to use a ball nose bit to do a rought cut. One of the first things, I cut on my machine was the gapes and leaves that was a model. I used a 0.25" end mill to do the rought cut and an 0.125" ball nose bit to do the two finish passes. When I was finished, it do not need to be sanded and there was lots of detail.

It all depends on how much detail your model has which can determine what size of ball nose bit you want to use.

[TimSchubach]

You reset the touchpad to an uncut spot on your material.
Cheers
Wolffie

Hi Wolffie,

It didn't dawn on me until just now that I could use an uncut spot. On all of my other projects, I've been setting my origin to the center of the piece instead of one of the corners. With a frame around the litho, the corners would be uncut - why I didn't think of that before I don't know.

Thanks

[Ms Wolffie]

Hi Tim
You do not have to use the origin for the plate, it only registers the height of the bit.
Cheers
Wolffie

[fixtureman]

I normally zero to my table but for lithos I zero to the top of the material. I find that if I zero to the top of the table it takes forever to render the litho and it will do an air cut before it cuts. I don't use a roughing pass any more either as there is so little that is being removed after the first plunge. I use a .062 ball nose end mill

[Dclifton2]

If your using mach3 there is a great screen set that does a semi tool change. It's called screen set 2010. There is a link on mach3 web site and works exceptionally well. It uses a second touch point.
Don Cliftom

[ssflyer]

I always z-zero to the table for lithos - It allows me to precisely control the minimum thickness of the material, without dealing with possible material thickness variations. I generally go for ~0.003-0.005" minimum. Also, I never get an aircut doing them, but I use Aspire. Perhaps PhotoVCarve is different in this respect?

[Keith Hodges]

You don't have to change bits between the rough pass and finish pass. I use .125 ball nose, using the step by step guide Tonydude gave you. On the rough pass I use the recommended 40% step over. Then on the finish pass, using the same bit, same z0 sitting, I use a 12% step over, with beautiful finish results. Keith Hodges

[calgrdnr]

I zero on top of material , I have had no problems . I see where Zero from table surface makes sense , but at one time someone was having problems with air cutting. so lost a lot of time. So I keep doing it from top of material .


I never do a rough cut. if you are cutting at the 45 degree angle (I set it to 315 so it starts at x0,y0) the bit will only do 1 plunge cut full size of bit the rest will be factor of your step- over, I use 10% or 8% depending on resolution I want. So at 10% of 0.125 you are only cutting at 0.0125 per line (1/10th of the bit diameter)

For the highest resolution picture/Lithophane I use 30 degree V bit but tell software it is a 0.030 ball nose. this bit comes to needle point.. it has broke just the very tip and is less then .030 still .. so at 10% it is only cutting 0.003 wide lines ... It gives excellent resolution ..... Of course will take over 4 times as long as a 0.125 bit to cut a Lithophane .

So in my opinion your are wasting time by doing a roughing cut at least in Corian . If your machine can handle it. I am sure carbide bit can handle the above procedure. I have cut many a Lithophane with no problem
you can always test with a small sample to see that it works . scroll down there is a tutorial with settings I use

for Aspire http://www.vectric.com/forum/viewtopic.php?f=28&t=12871
for PVC http://www.vectric.com/forum/viewtopic.php?f=7&t=7175

Kent

[BDM]

Tim,

Although there is nothing wrong with the Vectric method or Tonydudes, Kent's method of using the 30 degree v bit is so stupid simple, that it is hard to make a mistake. I've never had a problem using his method (at least with corian). Takes all the math calculations away and produces a fantastic result. But it doesn't hurt to try different methods and see which one you like.