|Home » Forums » CNC » Message||Login|
You are not logged in. Consider these WOODWEB Member advantages:
I’ve attached a picture of a chair leg (1 ½” x 6” x 48”) that I’m wanting to cut on my CNC. I running a Biesse Skill. I will be using Aspire software to cut the piece(s). I am looking for suggestions on what tooling and process(s) to use for this application?
What is material and thickness? Do you want to make one pass or several passes?
The material is 1 1/2" thick. I wold prefer 1 pass.
I don't think you can get a quality cut and cut that in one pass. It becomes too hard to hold in place and not burn up your tooling.
I would cut it out with a roughing bit then use a low helix spiral to finish the cut. probably 3/4" diameter bit if not larger.
I agree with Jason. Multiply passes is going to be better all the way around. I think hold down is going to be your biggest issue. We do have the slow spiral both in the ruffer and the finisher. A downcut will assist with holding if needed but and upcut is always better if you can use it.
Why a 3/4" Tool?
I think a 1/2" Dia tool should work fine. I think Jason was saying 3/4" for strength to keep from breaking on a single pass. The issue with that is it will want to push
If you can hold it well, 1/2 slow spiral upcut rougher 2 or 3 passes climb cut 800 IPM 0.020 oversize then one pass 1/2 compression spiral full depth final size conventional cut 250 IPM.
I find 3 passes at 800 IPM evacuates the chips better than 2 passes at say 500 IPM.
If you need to screw the piece down and then use 4 or 6 1 in long 3/8 thick tabs and band saw and trim the tabs offline.
If you have good hold down then 1/2" upcut spiral at 3 climb cut passes of just over 1/2" deep each. Use a .03" offset from the final part surface. Follow up with 2 passes with the same bit in a conventional direction at final part width.
If your hold down is questionable then use a downcut spiral to help prevent uplift on the part.
This has been what we've used for 6/4 and thicker blanks for our wood radius mouldings for many years. We're holding the parts with vacuum pods so use the downcut spiral bit to help in the holding power in most situations.
Sometimes we are so focused on using the CNC to cut a part that we lose site of alternative methods.
How about cut a template to that shape on the CNC, rough the part on a bandsaw and trim it using a bottom bearing and a straight cutter on a shaper. Double side tape the part to the template if you have to.
If I had to make that part I think that is how I would approach it. I happen to have all the equipment, heads and bearings to do it.
Before we got our CNC back in the late 90s we used to do exactly what you are suggesting. I even had a custom set of bearings made for the shaper that go from about 2 1/4" diameter all the way up to about 10" diameter. With a given cutter head we can flush or rabbet almost any sizing issue that we encounter.
Once we got the CNC we sent hundreds of curved moulding templates to the recycling station as the flushing/rabbeting offset shaper steps were no longer necessary. The CNC eliminated dealing with the templates, cutting on the bandsaw and the shaper bearing step. All in all this was a huge savings in time and labor.
However this process would have been worthwhile if we were just making one occasional moulding. Given our volume though the CNC was a significant improvement.
If the original poster is just making a few of these legs I agree that your suggestion is the way to go......especially if he isn't set up to do this type of thick cutting on the CNC. However if this is a large production run then he will be way ahead in sorting out the tooling/hold down issues.
We do these from a block that is about an inch or so longer than the finished part.
Make a fixture that locates the block with dowels and use Destaco clamps or similar to hold the block clamping on the excess portion. Cut as I suggested earlier using tabs. This is inexpensive to set up and has a quick load/unload cycle.