Whats the "proper" technique for cutting out 2D profiles on a cnc router?

[Zeppelin1007]

I know kind of an odd question guys...being christmas eve, i was trying to cut a few neat little doodads for family members..most of which use 2.5D milling...and simply different router bits...ball nose, corner round,2 flute straight cutter..

a problem ive run into here and there is, sometimes when cutting the outline of a part out, the router will fling it when its done..

or in the case of tonight...randomly decide to break the part in half! im going to guess a combo of vibration and crap wood...

for double sided parts usually i cut alittle of the outlining profile on the top side, then all the way through on the bottom side and leave one edge for last...at which the machine rapid back and fourth giving me plenty of time and room to gently remove the part once its free

i have milled from both sides and tried to do the "tabs"...with mixed results. or simply leave .05" and razor blade it out...then sand the sharp stuff off.

So whats the "proper" way? what if im only routing one side? seems tonight no matter what i did, ended in busted up parts...so seriously cleaning and such will commense tomorrow.

Similar Threads:

• LouieAtienza's "Dovetails on the Flat" Technique, take 1
• FastCut 2" end mill. 4 flutes 7-3/4" OAL, 4" cutting length. 1/2" radius, 79504
• Need Help!- Cutting a 7.1" circle from 0.5" thick 6061 alum - End Mill "loading up"
• "Open Source" Aluminum Extrusion Profiles

[rbraeking]

I do not cut to full depth so that the workpiece stays put. I usually make my cutouts using a 1/4 bit last leaving 1/8 depth uncut. This does 2 things.....saves cutting into the spoilboard and secures the part. When finished I cutout the part with a jigsaw or bandsaw then trim the remainder of the edge with a pattern bit on my shaper. Then I sand it smoothe on the stationary belt sander. Tabs work too but they have to be at least 3/16 thick and they take too much time to cut as the zed has to jump around them.

[ger21]

sometimes when cutting the outline of a part out, the router will fling it when its done.

That would be more of a workholding issue rather than cutting technique. Or at least a combination of the two.
I typically will leave a .005-.01" thick onion skin. This allows me to pop the part free by hand, and easily clean up with sandpaper. Sometimes, the part calls for more holding power, so I leave a thicker skin and clean it up with a laminate trim router with a flush bearing bit.

or in the case of tonight...randomly decide to break the part in half!

Without seeing the part, it's hard to say. While cutting technique could be the culprit, I'd again lean toward holding the parts still.

Solid wood can be a very tricky material to cut. Sometimes grain direction plays an important role.
In some cases, rather than creating single toolpaths around the perimeter of your parts, you might be better off cutting each side independently.

But, keeping your parts perfectly still is the one of the most important things. Whether you use tabs, onion skin, clamps, screws, or nails. If you need to manually hold the part or grab it while the machine is running, you need a better method.

[jm82792]

I bought 60 yards of 1" by 1/32" double stick tape that works incredibly well for holding down parts(too well at times, using too much means I will lift my 50LB table top machine off the ground. That and snap thinner parts) for $26 on ebay. Perhaps using a little bit of the tape(like 6" of tape per square to start) with your current work holding system would work.
There is definitely a bit of movement when using tape, but so far I've noticed good finish quality. If you want to do tabs perhaps you could simply edit the gcode with NCPLOT and simply select a few points, then raise them up?

Anyways here is what double stick tape is helping me do.
Edges come out polished, and everything cuts out well with the tape.

[fixtureman1]

I use tabs when I cut mine also I have a 3/16 flush cut bit that works great in a 1/4 kerf.

Flush Trim Bit with Miniature Ball Bearing Guide by Amana Tool

[adprinter]

I know kind of an odd question guys...being christmas eve, i was trying to cut a few neat little doodads for family members..most of which use 2.5D milling...and simply different router bits...ball nose, corner round,2 flute straight cutter..

a problem ive run into here and there is, sometimes when cutting the outline of a part out, the router will fling it when its done..

or in the case of tonight...randomly decide to break the part in half! im going to guess a combo of vibration and crap wood...

for double sided parts usually i cut alittle of the outlining profile on the top side, then all the way through on the bottom side and leave one edge for last...at which the machine rapid back and fourth giving me plenty of time and room to gently remove the part once its free

i have milled from both sides and tried to do the "tabs"...with mixed results. or simply leave .05" and razor blade it out...then sand the sharp stuff off.

So whats the "proper" way? what if im only routing one side? seems tonight no matter what i did, ended in busted up parts...so seriously cleaning and such will commense tomorrow.

I frequently use the following method:
Cut the profile to within maybe 0.010" of the bottom of the stock. Unclamp the stock from the table, flip it over, and for added support (to prevent splitting or cracking the wood), place it onto a piece of 1" thick foam rubber. Then clamp the stock back down normally. Next, I machine a pocket cut to Plane the remaining 0.010" of the stock to complete the profile cut out. Works for me.

[louieatienza]

I use both onion-skinning and tabs just fine. Amana makes a 1/4" flush trim bit that is perfect for most tab removal. With onion skinning you have to be careful with certain types of material, such as oak plywood, where you might pull the grain when "snapping" a part off; the 1/4" flush trim bit is a good option and eliminates a lot of hand work.

I cut a lot of G10 where the slug can trap and shatter the PCD bits I use. I used to run a drill op and put pilot holes in all the slugs, then screw them down to the spoilboard. Now, I just pocket them out, saving a lot of time in fixturing. I still have the parts screwed down through the bolt holes to keep them fixed.

In VCarve Pro you can position tabs literally wherever you want or need, so that you can put them in an inconspicuous or advantageous place. Another way is to profile cut leaving an onion skin, then do a finish pass with a smaller bit through; the smaller bit usually has less tendancy to "grab" a part. Another way would be to cut a fixture that elevates the waste and allows the parts to frop through. For some small parts I've even glued teh parts to scrap phenolic board with thick CA glue, then removed the part with acetone. For paint grade material I've also simply pinned the parts down with an 18ga pinner, but you have to be VERY CAREFUL not to hit a nail, or you'll ruin your bit and possibly send carbde flying.

[Zeppelin1007]

holy crap guys thanks! Ive been doing it wrong lol. Ill be resetting my machine up this week..took er down for a new years party. Eager to get millin again!

jm82, what CAM software did you do to get those 3D contours?

[louieatienza]

holy crap guys thanks! Ive been doing it wrong lol. Ill be resetting my machine up this week..took er down for a new years party. Eager to get millin again!

jm82, what CAM software did you do to get those 3D contours?

There's really no right or wrong way per se nore a matter of the best technique for the situation at hand. Sometimes it's a combination of techniques.