Blown edges in cedar letters

[cnc_works]

We hear off in the distance a quiet cry, it grows and grows until there is a full blown scream of panic and desparation.

Yup, that's me.

Most of the carving I have done is V carving with some raised letters in harder woods. I'm working on a 36" X 72" oval sign in western cedar and what you see is what I got.

A fresh 1/2" double edge end mill, resharpened, but it passes the thumbnail scrape test. 1200rpm, 90ipm, .25 stepover. .25 deep. You see the first cut, still on the raster with the 1/2" profile yet to come, with a planned 1/8" clean-up pass coming after to catch what the 1/2 bit doesn't. As you can see, corners and edges are being blown right out. No way will the profile cut clean up enough and I suspect not even if I climb cut everything.

Soooo, help!!!!!!!!!!!!!! please.

Donn

6054

6055


6056


6057

[scottcox]

Donn,

I'm no sign expert, but how about try a different toolpath stategy and do area clears or profiles. Select the insides of the letters first and area clear, then select the letter's outer vectors AND the outer oval, group them to create an area between the letters and the oval then area clear that with the offset option.

I think you'll get a lot cleaner letter edges than you would rastering.

Just an idea. Good luck.


6058

[Brady Watson]

1) Use a down-cut spiral as 1st choice or straight bit as 2nd choice.

2) Use a climb-mill toolpath strategy, not conventional.

-B

[elcruisr]

I've done many of these for sign shops and cedar is a pain! But, like Brady said, downcut spiral, climb cut profiles with a .040 finish pass and a very small chipload. The smaller chipload means more RPMS and lower tool life but, for me at least, has meant better letters in cedar. I also found a low helix polished O-flute plastics tool works pretty good in this stuff. Also keep some glue handy, You'll still have a chip to fix once in a while.....

[cnc_works]

OK, I think I have a 3/8" 2 flute downcut spiral, run it 16K, climbcut profiles, .040 finish.

What about feed speed and stepover? I'd sure like to go faster than 90ipm and it isn't coming close to working at that speed. But quality is first.

Does 50% stepover aggravate the situation? I mean, coming back on the conventional half of a raster cut, I could just hear and see the grain being split out in front of the cut. More...Less?

Lastly, would HDU be pretty well chip free in this application? Would you use the same bit and toolpathing? If so, I think I'll suggest this to my customer for the next job.

Thanks a lot for the hints.

Donn

[paco]

Donn,

if you intend to have those raised letters prism/beveled, start by profiling the letters with the V bit then pocket around with the end mill.

For straight cut, like Brady and Eric, climb cut rather than conventional.

[beacon14]

As Paco alludes to if you do the smallest profile pass first (you say you will use a 1/8" bit for final cleanup - run a profile pass around the letters with the 1/8" bit first) then when you use the larger bit for the hogging out there is no contact between the larger bit and the edges of the letters or the border. Make sure the larger toolpath has an offset from the letters to ensure no contact.

[frank]

Donn,

Is the error only in the Y axis? Check for a loose set screw on your pinion gear.

[paco]

Frank has point... but I think it's more type of wood and grain way related.

Almost all softwoods that I try cut that way did this. It need to be cut in climb fashion. More clean up but a least you got the part at the end.

[donchapman]

Western red cedar is one of the most difficult woods to rout cleanly, but it can be done and I've done many over the years.
Here's what has worked for me:
-Use only very sharp solid carbide downcut spiral bits.
-Take it slow and easy and in multiple steps.
-Start by using a 1/8" downcut spiral to outline your letters and graphics, but even here do so with multiple shallow steps down to the full depth of your background.
-Hog/Pocket out the remainder of the background with a larger diameter downcut spiral bit to reduce the remaining routing time
-10,000rpm @ 1.7ips is the typical slow speed at which I rout most western red cedar

It may be slow, but it beats destroying your sign blank and having to start all over again, and most of these 2D wood sign routing jobs are not that long anyway.

If you use the above methods you may still have some minor blowouts on small corner details, but nothing major.

[donchapman]

And yes use a climb direction of cut.

[knight_toolworks]

a rougher bit would work too. both cut most things without tearout.

[myxpykalix]

I suggest you give the guys at centurion tools a call, they seem to be pretty good with info on bits and might be able to help you. I saw a 1000% difference in my cuts due to the quality of their bits and they weren't much higher than the cheap crappy bits i used before.
http://www.centuriontools.com/
Phone 540.967.5402

[cnc_works]

Thanks for all the input. I've been slowed down by a serious accident that has me at half time at best so I haven't tried anything yet.

Spent my energy Friday gluing in patches. Ordered a couple downcut 1/8" from Hartlauer that will be in Monday. Love those guys, I can order before 3pm on one day and get the bits the next day. I discovered a 3/8" downcut in my bit collection, so I guess I'll be ready on Monday afternoon to try the suggestions.

Donn

[cnc_works]

Well, an update to the problem.

I'm sure there is still room for improvement, but here is the technique I used to get a result that pleased my client.

First, as David and others suggested I profiled the letters with a 1/8" downcut 2 flute bit in 3 passes to cut .27" using a climb cut 100ipm at 12000rpm. Nice cut, no chip blow out.

Then programmed a two tool area clear with a 3/8" downcut and a cleanout with the 1/8" downcut. Same feeds/speeds. Ran the cleanout with the 1/8" first, then used the 3/8" climb cut and offset toolpath for the real clearing. I lied to the program, telling it that the bit was a 7/16" so that it never contacted the letters at all. The problem with the 3/8" downcut was the bottom of the cut was pretty rough and the semi-random offset paths were rough and obvious.

Since the signs were two sided I had an opportunity to further improve my technique on the other side. Same 1/8" toolpath and cleanup, but the major clear was with a 7/16" upcut spiral running a raster toolpath. I also fibbed to the program telling it that the bit was 1/2" so it never got closer than 1/32" to the letters. The bottom cut was clean and smooth, virtually perfect.

The only problem I had was a very slight mismatch between the z heights of the cuts of the 1/8" and the 7/16" bit. A tiny ridge around the base of each letter. I suspect it may have been that I waited overnight between the profile and the cleanout cut and the wood moved slightly.

Total time of cut a little over six hours for both sides which meant that, if I ignore my learning time and patching time, my bid was right on the money and I should make a profit in the future. I have another similar sign to cut tomorrow and I think I will push the speeds just a little.

Thanks a again for the suggestions.

Donn