Routing MDF on CNC

[Making chips]

I have to router some parts out of MDF. This is one material that I do not have any experience with. I need to route through 1/2" sheet using a 3/8" carbide cutter. What flute number and configuration do I need? Straight, downshear, or upshear. I am hoping to be able to vacuum the part down on another sheet of MDF to hold it, but I am not too sure it will hold. Maybe I will need to make a spoilboard. The part looks like a 10" steering wheel. Any suggestions on feeds and speeds would be greatly appreciated. I have 7.3 kW spindles rated up to 24,000 rpm. I was thinking about 18,000 rpms with 400 ipm to start. What cut should I use as well? Climb or conventional.

Any input would be appreciated.

Thanks,

Paul

[jweinhold]

Paul,

I would recomend 2 wing down sheer tool. The down sheer will actually induce or aid you vacuum. 18,000 RPM and 400 IPM climb cut with a sloping lead in should be a good starting point. We machine 3/4" MDF with 1/2 tool at a 18,000 RPM and 480 IPM climb cut.


jweinhold

[ger21]

Conventional cut will give a better cut quality than climb cutting. At 400ipm, 15,000 rpm is better. And I'd use a 2 flute downcut spiral.

[Big-tex]

Conventional cut will give a better cut quality than climb cutting. At 400ipm, 15,000 rpm is better. And I'd use a 2 flute downcut spiral.

x2
Also cut material trapped in tool path will help to hold it in place.

[jweinhold]

Conventional cut will give a better cut quality than climb cutting. At 400ipm, 15,000 rpm is better. And I'd use a 2 flute downcut spiral.

Opinions vary we are cutting between 200 and 250 parts (10 to 14 sheets of MDF) a day. Now please understand I only have about 15 years of experance in working with MDF and at the height of the market we were producing 850 parts a day on average.

Test and find out what works best with your equipment and tool combination.

Good day,
Jeff

[Big-tex]

Vacuum should hold as surface of MDF is dense.
If you like to achieve clean cut on both sides with out chipping or blow outs use compression. Onsrud makes 3/8 compression tooling. It works fine for me.
Here is link to their catalog in pdf
https://www.onsrud.com/OC/pdf/OC-08CatalogR.pdf

Also if you look thaey have chip load charts and am sure you can figure based on that feeds and speeds. I find it very useful to get me started.

[jweinhold]

Big Tex you are 100% correct, when machining melamine backed material a compression tool does work best, raw MDF really doesn't seem to make a big diffrence. Onsrud's pdf will also definatly get you off to a good start.

[todd71]

One benefit to conventional milling vs climb milling is the cutter is pulling away from your material. Which if your part does move it wont "climb"
around causing gouges. It just pushes away.

[ger21]

If the part moves with conventional cutting, it usually gets sucked into the cutter, causing a lot more than just a gouge.

[todd71]

Use "tabs", if you need them, and there should be no problem either way.

[Big-tex]

Use "tabs", if you need them, and there should be no problem either way.

That works well. Also you may try to edgeband spoil board that will prevent vacuum leaking from least dense part of MDF. (= more vacuum)

[jweinhold]

Prior to installing new spoiler boards we cut them to size, drill and counter sink holes to secure the board to the router table. We then paint the edges and the counter sunk holes with 2 coats of tightbond glue. Its cheap pretty easy and you are good to go for the life of the board. After we position the part to be routed we then cover the rest of the spoiler board with plexiglass.