Bit for 1.5” length of cut in 2x8

[tomhartnett]

Tom: Thanks for the clarification. Should the Z zero routine still stop at about 1/2" above the z zero plate, or should it continue to max Z and then lower as Scott mentioned above?

when set up to recognize the Z prox it should go up to max Z like Scott mentioned.
Go to this file location (C:\SbParts\Custom\my_variables.sbc) and check the &my_hasZProx value - set it to 1 if not already.

I just recorded a video of the C3 and ZZero being run on a DT tool with Z prox enabled in case it helps, but I think we are on the same page.

-Tom H.

[johnsontoddr]

&my_hasZProx was set to 0 in my_variables.sbc

Just to be sure I didn't do anything wrong, I reran all of the initial set up files. That still didn't change the variable to 1. I then edited the file and manually changed the variable to 1, restarted SB3 and the Z zero routine did exactly as Scott described. That is the first time it has done that since I've had the machine (around 2 years or so).

So the Z Prox is now working and the Onsrud 52-367 4" bit with 2 1/8" CEL has plenty of clearance over a 2x as you can see in the photo.

Thanks to all of you for the suggestions and help.

IMG_6693.jpg

[coryatjohn]

I've cut 2x4's and their cousins many times on my SB and always use a regular run of the mill 1/4" upcut Onsrud (or similar) with a 1" LOC to do it. There is no need for anything fancy here. 2x stock is simple, soft pine. It cuts very easily. As long as the collet clears the wood, the bit can be used. I've many times dove below the cutting part of the bit without a hitch. I typically will use a 6 IPS and 14,000 RPM with .1" depth for this type of cut. If you don't see a plume of chips, you're probably going to have to get out the shopvac and lend a hand but the cut will still go ok.

If you're not cutting a hardwood like maple or oak, you can get away with a lot of shortcuts.

[johnsontoddr]

Just to follow up with this, here is the test cut I did tonight with the Onsrud 52-367 on a scrap 2x8. I did a conventional cut at 12500 RPM and 4 IPM with .5" depth of cut. This gave a calculated chip load of 0.0096" which is in the range recommended by Onsrud for .5" depth of cut. I thought there was a bit too much vibration while cutting at those settings and the finish was a bit rough as you can see. I may try a climb cut with the same .5" depth of cut, followed by a full depth conventional. I'm not that concerned about the rough finish, though since this is for an outdoor gazebo. However, I have 4 2x8's to cut this pattern on both ends and 13 2x4's to cut a simpler profile on, so I want the bit to last through those cuts. I also attached a photo after I routed a 3/8" radius cove using a hand router. I have some smaller parts I need to cut out and route a cove on, but so far I've not found a CNC bit to do it.

One downside of the long bit is that my vacuum was largely useless at picking up chips, because the bit extends quite far below the dust guard.

IMG_6696.jpgIMG_6698.jpgIMG_6699.jpg

[scottp55]

Vibration on the machine translates into the cut quality.
Seeing as we both have the same spindle, and almost the same machine....try being a little less aggressive for better cut quality until you know where your machine's Sweet Spots are?
Chiploads are only a rough starting point and are really made for Big machines/spindles in production environment for the most part.
Maybe better to go with the conservative rule of thumb of pass depth equals half Diameter of the bit.
Feed on a wood you haven't cut before...good initial speed is 1.5 IPS...and then tweak your RPM's until it sounds good/chips are small but still chips/ and bit is room temp(or very slightly warm) at end of cut....THEN increase feed/speed together proportionally until cut quality suffers...and then back off about 10%.
For dense hardwoods and exotics I haven't cut before, I use 1/2Diameter and .8IPS as a starting point.
I found this helpful when I first started;
https://www.precisebits.com/tutorial...s_n_speeds.htm

A friend of mine with a Desktop just bought a long surfacing bit...same problem with the 2" standard dust foot bristles...lots of threads on here for ordering longer bristles, and I recommended possibly using spacers...BUT he took a pic and sent to Shopbot and asked if they made a 3"bristle for the Desktop....They made him the same exact dustfoot, but with 3" bristles for a $100..which was worth it for him at this point with orders coming in right now. Maybe?
scott

[coryatjohn]

.5" depth is way too aggressive. Unless you are in a production shop with a cast iron machine, that wouldn't really be a good depth. I personally never cut more than 50% of the diameter of the bit and will very often use 33% or less if I want a quality cut. If you hear the machine screaming at you, you're being too aggressive. Let your machine tell you when you've got it right.

Another issue is holddown. When being so aggressive, you have to keep the material perfectly still and held down tight. That is very hard with a light wood like pine. Carefully examine your holddown strategy and be sure that the material will not budge, buckle, jump, jiggle or move even 0.01" during the cut or you will have tearout and generally a poor cut or worse, broken bits.

A good bit cutting right will last 10+ hours. It is very hard to ruin a bit that's being used right.

[johnsontoddr]

Downloaded a GWizard trial and it also says I was way too aggressive. It recommended 10001 RPMs at 0.79 ips with a 0.25" depth of cut. That was at 25% finish on the Tortoise Hare Slider. A test cut at those settings definitely came out smoother, but I didn't like the sound--kind of a rumbly, low pitch, not a high whine. The bit was just slightly warm to the touch.