Cedar splitting issues

[Zoinac]

I have been following along with Eric's techniques for making cedar signs. I keep running into problems with my cuts though. I was hoping that you guys could give me some pointers to correct the problem I'm having.

Every time I cut a file the cedar splinters horribly. Where it doesn't splinter I get lots of fuzzies and flecks left behind- which causes the ink to bleed sideways into the wood.
Here is an example:

Cedar fail (http://i.imgur.com/B1pVz.jpg)

I cut it at 2IPS (down from 3IPS, made no difference) with a brand new 60 degree V bit, I cut conventional direction, offset , flat bottom depth of 0.2" (at 19k rpm, I tried 16k as well)
I did the clearing with a 1/8" down cut, which didn't leave a single piece of fuzz or junk left behind. It's all in the V-carve.

I suspect its a feed/speed issue. My endmills all cut perfectly- but the v-bit leaves a lot to be desired.

[bleeth]

Manufacturer and part number of the V bit?
Speed of Spindle/router?

[bob_s]

try it as a climb cut - I had the same problem on a lot of specialty moldings cut from cypress and alder. Climb cutting generally works great.
I still need to add blocking on some cuts as they clear the wood and turn from cutting end grain to edge grain if the wood is cut narrow enough for the bit to exit the edge. In some cases try to leave 20 thousands and then come back with a conventional cut - it just depends

[ajf]

Before I cut cedar, I seal the cedar with 2 to 3 coates of clear sealer. Then I usually use a feed rate of no more than 50 ipm. This reduces most of the splintering. After the cutting is finisihed I then seal the cuts with clear sealer to prevent the bleed out. I then paint the lettering with the desired colours. It seems to work for me.

[dlcw]

When doing signs (v-carving, profiling, cutting out, etc.) I always remove most of the material using a climb cut. The final cut (about 1/32") is done in a conventional direction. For v-carving into the wood (letters, graphics, etc.) I run my spindle at 18K rpm with a 1 IPS feedrate. This produces really clean cuts in the wood.

I run a lot of cedar, pine, alder and hickory through my machine and the above feeds and speed seem to work well. I use an Amana 1/2" shank with replaceable angle blades for my v-carving. They are really easy to run across a ceramic stone to hone them to super sharp. I use ceramic for honing as this is what I use to sharpen and hone my chip carving knives to be incredibly sharp (thank you Wayne Barton).

[chiloquinruss]

In what order did you do the toolpaths? Did you do the clean out first and then do the vcarve? If so try reversing the order and do the vcarve first then do the cleanout allowing for a little offset. Might help. I also do a couple of coats of sealer before cutting. Russ

[Zoinac]

I'll certainly try doing a climb cut first.

Don,
In aspire, how to you approach setting it up to cut the last 1/32" separately. In most tool paths there is an offset box- not in v-carve path. Do you actually create offset vectors, or do you just tell it to come back with a slightly lower start depth?


edit:
Well, I re-cut the cedar using a CMT 90 degree bit, slowed down. Much better results. Still the occasional chip here and there. But I suspect that the majority of the problems were caused by a cheap bit issue.

[dlcw]

Aron,

I create two tool paths. The first one cuts to within 1/32" desired depth in a climb direction. Then I create a second tool path that starts at the ending depth of the first tool path and does the finishing cut in a conventional direction. Since the two paths use the same tool, you can save them both in one file and when you run the file it cuts both directions for you. This method works in Partworks, VCarve Pro and Aspire. I suspect it will work in just about any CAM software because it is so simple.

[bleeth]

There are a variety of better quality bits that we have all learned make more sense to use for our shopbots. Amana, Whiteside, Centurian, and Onsrud are some general favorites. There are others but typically Freud, Grizzly, CMT and other popular priced bits made primarily for hand routers don't do it with a CNC. You want to use solid carbide and not carbide edge. They are more accurate and have a superior grade of carbide. Using a 12-40K machine with a cheap bit in it just doesn't cut it. Pun intended;)

[joe]

I'm with Dave on this one.

Last week I was doing some V carving and the results were poor. You'd think, after all these years, I'd be able to look at a bit and tell if it's sharp. Well, I can't. After sending these off for sharpening it was amazing. You know, it only cost $3.00 each. These were high dollar Gerber bits and I dreaded sending them off. See I keep learning.

My least favorite V's are the 60's because it's hard to read anything after the carving. Sometimes a 90 is even too steep for me.

Prior to carving, I'll usually make several test cuts. V carving is a relative quick process and the difference in image quality will be delicate. This is where I slow down. I seldom, if ever, end up using the zero the machine comes up with. The machine is accurate but it doesn't inteperate font thickness, stroke.

With the V process letter stroke is just as important as letter height. Sometimes it's even more important.

Joe Crumley
www.normansignco.com


+

[David Iannone]

Joe,
Your point is very interesting. I have had signs I previewed in VCP that I liked the depth and width of the V-carve. When I carve them they don't look "exactly" like the preview. They don't look bad either and it hasn't been anything the customer picked up on, just a slight difference that I pick up on. I always figured it was possible my v-bit not setup correctly. I rarely do test cuts either, but what you are saying makes perfect sense. I will have to do some sample V-Carves in various fonts for my sales area. As always thanks for your wealth of knowledge.

Dave