Upcoming Project

[parkin79]

So my office is having me make them a 3x6 map of the world to hang in our reception area. Its going to look something like the attached image. My question is, i will be using a 46180 CNC Solid Carbide Compression Spiral 1/8 Dia x 13/16 x 1/8 Inch Shank. Is this the right bit for this type of project? does it need to be a compression bit? i know if used properly it will reduce sanding and overall cleanup. Next i keep reading reviews on these bits and most people say how great they are, while others complain how they break, is that because they are being to aggressive with the speeds?

Any tips before i start this would be appreciated.

Attachments:

[redwood]

I don't think that you mention what material you are using nor the thickness.

[parkin79]

The map will be cut on 1/2 inch birch plywood.

[Deleted]

That bit will work for your project but keep in mind that to have both top and bottom faces work well with the bit you'll be doing a full depth of cut with a fairly small bit so the feed rate will be low to minimize deflection. If you have the option of using a larger diameter compression bit then it will be significantly stronger and resistant to deflection and thus breaking.

[grg]

Oct 6, 2018 22:50:54 GMT -5 @fean said:

That bit will work for your project but keep in mind that to have both top and bottom faces work well with the bit you'll be doing a full depth of cut with a fairly small bit so the feed rate will be low to minimize deflection. If you have the option of using a larger diameter compression bit then it will be significantly stronger and resistant to deflection and thus breaking.

I see this conception about compression bits all the time - which is probably why people break them a lot.  In reality, each pass only needs to bury the up-cut part of the bit below the surface of the material and you can make several passes.  For that bit in question, the up-cut is 7/32" long.  Respectively, each pass just needs to be 1/4" deep.  That's still pretty deep for a 1/8" bit in plywood (I try to max out at bit diameter) but it's certainly better than trying to go full depth with it. 

I use 1/4" compression bits in birch plywood a lot with multiple passes.  I frequently use this 1/4" bit - it has a 5/32" up-cut portion and I make passes of 1/4" in plywood with it with good results.

[parkin79]

Thanks guys are all the suggestions. I'll be starting at this project this week so I'll keep you guys up to date on how it works out thanks.

[Deleted]

Oct 7, 2018 9:28:48 GMT -5 grg said:

Oct 6, 2018 22:50:54 GMT -5 @fean said:

That bit will work for your project but keep in mind that to have both top and bottom faces work well with the bit you'll be doing a full depth of cut with a fairly small bit so the feed rate will be low to minimize deflection. If you have the option of using a larger diameter compression bit then it will be significantly stronger and resistant to deflection and thus breaking.

I see this conception about compression bits all the time - which is probably why people break them a lot.  In reality, each pass only needs to bury the up-cut part of the bit below the surface of the material and you can make several passes.  For that bit in question, the up-cut is 7/32" long.  Respectively, each pass just needs to be 1/4" deep.  That's still pretty deep for a 1/8" bit in plywood (I try to max out at bit diameter) but it's certainly better than trying to go full depth with it. 

I use 1/4" compression bits in birch plywood a lot with multiple passes.  I frequently use this 1/4" bit - it has a 5/32" up-cut portion and I make passes of 1/4" in plywood with it with good results.

You can cut with this 1/8" bit for full depth, you'll just have to feed pretty slow because of the deflection limit of the tool. If there is too much deflection, the tool will snap, as you approach the limit your cut quality drops too. Also keep in mind that a 1/8" bit in a 1/2" board will have a tougher time clearing chips than a larger diameter one, especially because of the down cut profile at the top of the bit. The rigidity of the tool goes up at the 4th power of the diameter thus if you go from this 1/8" tool to this 1/4" tool:

www.amanatool.com/46180-cnc-solid-carbide-compression-spiral-1-8-dia-x-13-16-x-1-8-inch-shank.html?ff=1&fp=10796

You'll increase the rigidity, and decrease the deflection by a factor of 16. You can get a hint of this from the Speed and Feed chart that shows the comparative increase in feed rate and tooth load if you look at the various diameter tools available:

www.amanatool.com/pub/media/productattachments/Solid-Carbide-Compression-Spirals-v4.pdf

While the 1/8" will get you more detail, you might consider switching to the 1/4" if your detail of cut allows. Another option would be to use a 1/4" bit to make a profile 3/8" deep offset say 0.05" so that when you're using the 1/8" it isn't doing a full width of cut for the full depth and there would be plenty of room for chip removal, all of which would help deflection substantially. Recutting of chips is also tough on tools because of heat build up.

Since deflection also increases at the cube of the stick out length you'll also want to have as little bit sticking out as possible for such a small one.

Don't forget to add lead-ins and outs so that you can add ramps your plunge moves outside your actual profile cut area.

[traindriver]

Would it make sense to rough cut the pieces with a larger diameter downcut bit (since the only surface you really care about is the top one) on a path slightly larger than what you want, then clean up with the 1/8th inch compression bit in order to have the desired definition without the worry of breaking it?

[parkin79]

I was actually setting up my file that way and may go that route.