Cutting hardwood

Bill OConnell · Post by **Bill OConnell** » Thu, Aug 25 2005, 10:16AM

We are making two 5.5\" x 4.5\" ovals that will terminate a handrail into a wall. We are profiling it using roundnose cutters and have tested our program out on MDF.

Now comes the fun part. We went to cut the first piece out of oak and it threw the part.

Questions:
1) How deep should we limit our plunge on each pass? We were plunging 0.25\" but seeing some tear out on the surface and when we went to outline the part it threw it.

2) We are using a 10HP router with variable speed. How slow can that reasonably be operated? To avoid some lateral stress we want to slow the feed rate and know we should slow the router speed at the same time to avoid overheating the bit. What is the lower limit?

3) What recommendations do you have for holding hardwood parts if the vacuum doesn't get it done?

Your suggestions are appreciated.[/list]

David Hall · Post by **David Hall** » Thu, Aug 25 2005, 11:56AM

Forget trying to hold this with univeral vacuum through a spoil board. It won't work. Since you've only got two to do, get out the double sided tape and tape it to your spoilboard. But do turn on the vacuum when you run the piece (the vacuum changes the Z position of your spoilboard. Cover the unused portion of the table. You should be climb cutting hardwood to get a clean edge. Tape the off fall down too or be ready to duck.

What bit are you using for the outline? How thick is the material?

The bit manufacturer is your best source for feed rate and spindle speed recommendations.

Bill OConnell · Post by **Bill OConnell** » Thu, Aug 25 2005, 12:12PM

The material is 3/4\" stock.

I was using a 3 flute 1/2\" rough cutting bit for the outline.

Tooling manufacturers have been very helpful in providing spindle speed vs. feed rate calculations, but I was asking if there is some minimum speed on the 10HP below which you start losing power.

Forrest Chapman · Post by **Forrest Chapman** » Thu, Aug 25 2005, 8:55PM

Hey Bill,

Maybe this will help it works well for us. We use a 1/4\" upshear bit with 1\" cutting edge. RPM's at 18000 and IPM at 150 to 180. Cut 1/4\" per pass. Set up a board or boards to surround your oak blank which should be a little larger than the finished size. Sometimes when I need a quick fixture I just staple a few blocks around the part. As it cuts the last pass there is usually enough trash in the space to hold it center. You probably will not want to run your dust collector as it may pick up the part on the final pass. Try to make your bit as short as possible to avoid flexing. Also make sure to keep your part about 6\" off the edge of the table. Hope this helps.

PS. Its going to sing!

Forrest

Bill OConnell · Post by **Bill OConnell** » Fri, Aug 26 2005, 8:37AM

Forrest,

Great suggestions

I will definitely add them to my tool bag.

The client came by yesterday, so here is what we did. I re-wrote the program to plunge 1/8\" per pass, not only for the profiling but for the outline as well. We decided to leave a 0.02 skin on the bottom and just sand it off. For hold down, we screwed the board through the wasteboard and into the spoil board with 1 1/4 screws, being extra careful not to go into the tool path.

When it was getting moving to cut the secong piece, I didn't like how close it was to the first so I dialed the machine down to stop it and cancelled the program. I changed my second fixture location and re-ran the program but nothing happened. I had forgotten to turn the override back up from zero.

I wish that didn't happen in front of the customer.

Overall, it worked. I prefer some of the suggestions I have gotten from the forum and will use them going forward. Thanks to all.

Regards,
Bill

Jody Wilmes · Post by **Jody Wilmes** » Mon, Aug 29 2005, 10:30AM

In most cases I machine hardwood @ 18000 RPM...adjusting feedrate accordingly. Typically I'll program the feedrate high, then use the FeedRate OverRide Knob to slow it down. Once the best Feedrate is found, I do a search/replace to correct the program feedrates.
With the exception of cherry, usually I climb cut. I know some people conventional cut to get rid of any 'fuzz'. This works on certain plywoods as well...but beware of blowouts, etc.
Depth of cuts depend on the size and thickness of your part. Typically, I plunge the same amount (maybe a little more) as the diameter of the cutter. Cutter size also has a lot to do with it. A 1/2\" cutter produces more load on a part than a 3/8\" cutter...increasing the chance of part movement. Leaving a skin on the part will decrease the chance of movement, which you can machine off last.
If you do have only a few parts to machine, I would also suggest the double-sided tape method mentioned above. It'll be quicker than fighting a vacuum issue.

Jeff Norris · Post by **Jeff Norris** » Tue, Aug 30 2005, 5:02PM

all double sided tape is not the same, i have been using double sided duct tape, works great. carpet tape works good too.