PDA

View Full Version : How do I successfully run MDF with fine details on a ShopBot PRS Alpha?



jwatte
12-24-2012, 12:36 AM
I'm trying to make a plug for vacuum forming a part, and was thinking I could build it in a 3D modeling program, export to STL, vectorize in Cut3D, and then route in some thick MDF to create the plug.

It all worked very well, except when trying to route the MDF, it keeps slicing apart / de-laminating along horizontal planes.

My details are about 6 mm in size with about 10 mm stick-up above a more supporting surface.
I'm using a 0.5" HSS roughing end mill for the roughing pass, with 0.3" cut depth, 6,000 rpm, and 100 ipm feed rate.
I'm using a 0.25" carbide ball point end mill for the finishing pass, with 0.06" cut depth, 10% stepover, 12,000 rpm and 80 ipm feed rate.

Plunge rates are 1/2 of feed rates, but plunging doesn't seem to do any damage, only feeding into the thinner sections of the plug.

The roughing mill and the ball point both do damage to thinner parts, but the roughing mill is worse (for probably obvious reasons.) I'm coming at this from CNC milling aluminum, which is a somewhat more solid material than MDF, so any hints I can get would be appreciated!

jharvey407
12-24-2012, 07:18 AM
I'm trying to make a plug for vacuum forming a part, and was thinking I could build it in a 3D modeling program, export to STL, vectorize in Cut3D, and then route in some thick MDF to create the plug.

It all worked very well, except when trying to route the MDF, it keeps slicing apart / de-laminating along horizontal planes.

My details are about 6 mm in size with about 10 mm stick-up above a more supporting surface.
I'm using a 0.5" HSS roughing end mill for the roughing pass, with 0.3" cut depth, 6,000 rpm, and 100 ipm feed rate.
I'm using a 0.25" carbide ball point end mill for the finishing pass, with 0.06" cut depth, 10% stepover, 12,000 rpm and 80 ipm feed rate.

Plunge rates are 1/2 of feed rates, but plunging doesn't seem to do any damage, only feeding into the thinner sections of the plug.

The roughing mill and the ball point both do damage to thinner parts, but the roughing mill is worse (for probably obvious reasons.) I'm coming at this from CNC milling aluminum, which is a somewhat more solid material than MDF, so any hints I can get would be appreciated!

This problem is not uncommon. Once the top layer is milled off of the MDF it will have a tendency to 'flake' off, especially around small details. You may be able to avoid this by using a straight flute or down cut end mill.

The other option would be to use foam for the plug.

James

ger21
12-24-2012, 08:49 AM
I'm using a 0.5" HSS roughing end mill for the roughing pass, with 0.3" cut depth, 6,000 rpm, and 100 ipm feed rate.
First, switch to carbide. HSS will dull rapidly in MDF, and put more force on the material, causing increased breakage.

Tall, thin features in MDF are extremely fragile, as the core is very weak. Your best bet is probably to take shallower passes. I'd try 400ipm, 16,000 rpm, and .1 depth of cut. It should take about the same time, but with less breakage.
If that still doesn't work, then try roughing with a ballnose bit, which will leave a thicker, stronger base on your features.

What's the total thickness of the blank? You may be better off with a finish pass only, with the stepover at 6-8%. You'll only be removing ~.02"/pass. I know a lot of guys use this technique when carving hardwoods, using a tapered ball tool. If you start at the surface, or outside the material, the tool never removes much material, and is strong enough to handle it.

jwatte
12-24-2012, 01:26 PM
The other option would be to use foam for the plug.


Thanks for the advise!

Is there a particular brand or kind that might work well?

jwatte
12-24-2012, 01:29 PM
First, switch to carbide. HSS will dull rapidly in MDF


I don't have a carbide rougher, but perhaps a separate roughing mill isn't important for softer materials?


try roughing with a ballnose bit, which will leave a thicker, stronger base on your features

Also sounds worth trying!


What's the total thickness of the blank? You may be better off with a finish pass only

It's two inches, about 10x4 inches cutout area. Not very big, but doing finishing only would take a long time.