Bit for 1.5” length of cut in 2x8

[johnsontoddr]

I’m looking for suggestions on what bit I can use to cut a decorative end pattern on a 2x8 using my Desktop Max. I have the starter bit set, but it doesn’t look like I can cut that deep with any of those bits. As I move to longer bits I’m not sure what the max bit length of Max is. The specs seem to indicate a maximum cut depth of 3.5”.

[Tim Lucas]

try www.vortextool.com not cheep but good and sharp

Tim

[johnsontoddr]

try www.vortextool.com not cheep but good and sharp

Tim

The problem is that I'm not sure what length and width bit I should use. I assume a .5 inch diameter bit would be better to help with deflection, but I'm not sure how long an overall bit I can use in the Desktop Max with the spindle.

[Martin Reid]

Dear Johnsontoddr

The maximum length of bit and the maximum depth of cut can be calculated as shown on the attached image.

31365

The width of the bit will be a proportion of the length calculated by the manufacturer. If you think deflection will be an issue then slow the feed rate and reduce the depth of cut. You can hear a deflecting cutter 'singing' and if you don't do anything it will only break and take the collet with it. Some people don't change the collet after a breakage but that is a false economy.

Anyway best of luck
Sincerely and in good faith
Martin

PS further info on worn collets for those interested
http://www.talkshopbot.com/forum/showthread.php?24099-Tooling-marks-Buddy-Prs&p=198322#post198322

[Tim Lucas]

The problem is that I'm not sure what length and width bit I should use. I assume a .5 inch diameter bit would be better to help with deflection, but I'm not sure how long an overall bit I can use in the Desktop Max with the spindle.

I have a need to cut thick cedar for counter tops and such up to about 2 1/2" so i purchased this from Vortex Product #: 1265
DESCRIPTION: SC DE Upcut Finisher
CED: 1/2
CEL: 2 1/8
SHK DIA: 1/2
OAL: 4

my z can retract high enough to get the bit (about 3 1/4" sticking out of the router) above the material and not hit any dust collection and such, so i can use it.
look at your machine place a chunk of 2x8 on your table raise your z almost all the way up and see how much room you have then go from there.

The 1/2" bit is twice as strong as the 1/4" and when working with longer bits I would suggest using the 1/2" - they do have 3/8" bits but i dont have a collet for them.

hope this helps
Tim

[johnsontoddr]

Thanks for the suggestions. I raised the spindle up to near max Z with a 2.5 inch long compression bit installed (the longest I have). It looks like there is plenty of room for the 4" long Onsrud 52-367 to clear a 2x8, so I ordered that to try. Its cutting length is 2.12 inches, so plenty of length for a 2x8. To minimize deflection I will use multiple .5 inch depth cuts and start with Onsrud's recommended chipload for the bit in softwood.

[tomhartnett]

When you end up making the cuts/files, keep an eye out for your safe-z heights and pull-ups. With 2.12" CL and a 2" board (plus 0.5" spoil/base) you are at 4.5" or so taken up of your 5.5" Z movement. So you may have less than an inch of pull-up/space to work with above your material before topping out the Z.
The place to check in SB3 is under Values->Cutter Values (Safe Z pull-up - defaulted to 1") and if you are using VCarve/Aspire you'll find a Home/Start position -

31383

that includes a Z location (which will be where the tool goes at the start and end of the cut file). Make sure these values are within your working Z space where the Z won't top out during the operation.

-Tom H.

[johnsontoddr]

Very good points. I use Fusion 360, which allows me to set a clearance and retract height, but I'll also need to be sure that the Home point set in the Shopbot app can handle the longer bit. A 2x8 is only 1.75 inches thick so I think if I'm careful with all this it should work.

[scottp55]

Tom made great points(and beat me to it):)
Does your machine have an upper Z limit switch that prevents you from "Topping Out"...or do you hard stop when raising bit with keypad?
Topping out can have some rather dramatic movements if your not aware of it!
When working with my Desktop, VC Safe-Z pullup has been critical.
Just thought I'd toss a pic in....also maybe start directly over the workpiece the first time with the keypad in case you forgot something.
Jogging into the side of the workpiece at depth can make you spit coffee on your keyboard! :)
scott

VC is also nice when prototyping a thinner workpiece with it set at 2"....then you can run a few lines to make sure it's cutting right...hip Spacebar for a pause, and get your dustfoot on(spacebar pause kicks it out of the Vectric, and into the SB3 parameters)

[johnsontoddr]

I don't have a z proxy switch, though I do have the cut out bracket that could easily take one. I'll be sure to carefully set the safe-Z pullup to end above the material. I will try an air cut without a bit or material after I think I've got the settings dialed in.

[scottp55]

A friend had one of the first Max's out, and since it didn't match any of my pics...he called Frank.
ZProx just didn't look like it, BUT it was there(see first 2 pics).
So pretty sure yours does also.
Make sure that in VN , limit switches are turned on.
In TS (Tool Setup), make sure you checkmark the box "I have Z-prox"

That also changes the Z-Zeroing routine so that it double taps the plate,retracts to SB3 safe Z pullup and pauses,retracts to upper Z limit switch, then goes down .125"....MUCH better for installing dust foot then, and reasonably sure you wont hit material or clamps.

MUCH more reassuring when you know the machine won't top out, and will simply Stop if your setting are wrong:)
scott

Oh..ignore the other settings in VNpic...from this laptop that has never touched the machine.

[johnsontoddr]

Thanks Scott. You are correct. I have the Z Prox and when I raise the spindle up to near its limit, the switch triggers input 3. However, in Shopbot setup I do not have an option for telling SB3 that I have a Z Prox. I also discovered that in VN Limit checking was off and only switch 3 (for Z) shows NRM Open Limit, the rest say Standard Switch. My understanding is that all of the limit switches are connected in parallel to input 3, so that should be fine. My XY limit routine works fine, so I assume the machine can see those limits. Not sure why I don't have the option to tell SB3 that I have Z Prox.

[guitarwes]

Just FYI, Centurion Tools has a 1/2" spiral bit with a 1/2" shank with a 1.5" length of cut. Works great for me for 2X stuff and is not as long as some of the other bits.

[scottp55]

Not sure:(
Maybe because all Max's have it, it's defaulted?
Shouldn't think that would be it though.
Does Z-Zero routine run like I described?
If not, and no option for Z prox is in TS, then maybe get machine started/phone charged/ and call Tech?
When in keypad, and press and HOLD arrow up key for Z...it should simply Stop if prox is working.
Only way to hit a hard stop on our two Desktops, is if arrow key is "Tapped"...then it can hit the prox, but subsequent tapping can cause it to go by the prox.
Sorry not more help:(
scott

[tomhartnett]

It's slightly hidden in SB3 as it becomes part of the my_variables file and not the usual .ini file that stores our other settings (like switch modes). AND, we changed the way it was displayed in SB3 version 3.8.44 where it doesn't appear in [TS], so if you have 3.8.44 or newer, ignore the next part and skip ahead:

You'll find it under Tools->ShopBot Setup, in the first step with the check boxes you should find the Z prox setting like in the 4th picture of Scott's post.

Newer SB3 version - it gets loaded with the MAX setting file when you select it upon install or [UR] so you don't have to tell it specially that you have one, since it is a default on all the DT tools.

-Tom H.

[johnsontoddr]

Scott: The machine now stops when the Z prox is reached. However, the Z-Zero routine just stops at Safe Z, so the control software clearly doesn't think the Z prox is there. I will keep debugging. Perhaps I need to completely uninstall and reinstall the software. I just installed the latest version yesterday, but did not uninstall before doing so.

[johnsontoddr]

With a 1.5" length of cut can you cut down a little lower than 1.5", assuming the bit extends from the collet a bit more? I tried to look this up, but could not find a clear answer.

[tomhartnett]

All depends on the the edge length and the type of cut, if the CEL ends at 1.5" and you try to cut 1.51" of material at a time you're pretty much guaranteed to break that bit, but if you don't cut more than 1.5" at a time you certainly could exceed that depth of cut (until you hit the collet or head). This can be bad practice as the chips will not clear as well (again depending on the type of cut).

A kind of easy way to think about it, you can drill a 3" deep hole with a router bit that only has 1" of CE but 3" of overall exposed length, but you can't then move in the XY direction and cut that much material, but you could pick up the router, move it over and drill another 3" deep hole, repeat it and eventually you would have a shape or your cut complete.

this thread kinda does OK at talking about it: https://www.cnczone.com/forums/archive/index.php/t-152755.html

-Tom H.

[johnsontoddr]

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?

[guitarwes]

If you make multiple passes you can cut deeper than the CEL as long at the passes are not deeper than the length from the bottom of the collet to the end of the bit.
I haven't broken a bit yet. If you cut full depth in 1 pass, then no, you can't cut deeper than the CEL.

[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.

31393

[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.

314023140131403

[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/tutorials/calibrating_feeds_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.