Tiling - First time 4x8' Workbench Top

Hi Guys, I’m almost back up and running; (moving during COVID was quite the ordeal). Anyway, I’m building an elaborate 4x8’ benchtop and to do it I’m going to need to tile 2qty 25"x 98" pieces of Birch Butherblock top stock then join them together post milling.

Given this is about $500 in stock I wanted to run by the tiling procedure with you and make sure that it wont end in tears. So you know… the relative position of these holes in a grid is very important for certain jigs/tools to work properly with them. Precision is Paramount.


  1. I’ve watched a few tutorials on youtube where they zero X & Y using the midpoint on the stock… but I think it would be a better (more accurate) idea to use the locator pin hole created during each tiling procedure to RE-ZERO X & Y by plunging the bit into the locator pin hole…? (it’s pretty close to a 1/4" hole).

  2. I often see people drill into the spoil board first to create the locator pin holes, my approach was to square the stock on the spoilboard first, then drill THROUGH my stock into my spoilboard to create the locator pin holes; that way I have more control over pin-to-stock alignment… am I correct on both of these?

  3. I don’t understand the point of overlapping my containment boundary.

  4. It would be handy to puts a chamfer on all of those holes using a V-Bit. But that would mean a tool-change… So I’m leaning toward doing this by hand with a large countersink bit. Let me know if you think it’s worth it.

Here’s the F360 File for with my procedures. I also am out of practice with toolpaths kindly glance over them to make sure it’s as riding a bike as it feels.


I really like using the locator pin holes for flip operations and plan on doing the same when I do more tiling stuff. Usually with those type of procedures you’d want to use the router to drill out the pins for the next operation as part of the current operation, but if you have concerns about not wanting those pin holes in certain parts of the stock I can see drilling through the stock and then use the stock to drill spoilboard working well. The stock should guide the drillbit so you wont have much play on angles (I think?)

I think doing a chamfer would be best done by getting a chamfer bit for the router and do it by hand.
(something like this: https://www.amazon.com/Whiteside-Router-Bits-2306-45-Degree/dp/B001CGYOTY)


What about milling a template that you could use with a handheld router and bushing?

Hi Neil, they actually make this… https://www.woodpeck.com/hole-boring-jig-2019.html

I’ve used it… and it’s not as good as the results when I use the same pattern on my Spoilboard see below…


Get you a bundle of “crying towels” and get ready! :smiley:

I’m curious (from the standpoint of keeping your tears at bay) about which jigs/tools for a workbench require more tolerance than you can get with a 24" square template? I’ve seen clamping systems, but not jigs that would use multiple workbench holes.

The results aren’t as good or the pattern?
It’s on my list to make a small mft-style table, so I’m soaking in information.


I found that the holes done with that jig (which is in my mind is top-of-the line) were sometimes too tight… sometimes too loose… sometimes at a slight angle, and by the end of doing a 4x8 MDF top you could tell that they weren’t perfectly 96mm apart when viewed through the holes in the jig… (this could have had something to do with the MDF changing/warping/shifting or more likely operator error).

If I’m honest, I’m over-engineering more than anything, but heres a good example if you wanted to approach cross cutting long boards in this fashion. If your holes are half a mil out of square so will your be your cross cut.


So, you’re trying (crying? :smiley: ) in 8 ft. to keep 0.0005" tolerance? (Or even 4 ft.?) I don’t know how you will do this, let alone with your CNC.

No, I’m just trying to get the best result with the tools I have at my disposal; having tried the jig method the shapeoko is better. Further, I’m just looking for feedback on my tiling procedures, toolpaths, and approach to an unfamiliar process so that I don’t have an “oh-shit” moment with an expensive piece of stock after not running my S3 for 4 months.

Also… half of a mm is .02"… well within what the XXL can do (when not tiling).

EDIT: ah i c, yes… half of a MM not an actual “mil”


@neilferreri I’m about 4 tiles through the first half of the workbench and I would recommend you go with a jig if doing anything excessively long/big. Something is out of square by about 1.5mm over 4feet… it could be my rip cut on the stock or it could be the Shapeoko itself. I have enough overhang that I’ll be able to fix that since I’m being careful to keep all the holes in alignment to themselves, but overall tiling for something like this isn’t any more accurate then the woodpeekers jig.

Also, while I’m not in tears… I did have a Z-height loss issue (not a loose bit) when machining one of the holes… so now I have a nasty gash I have to fill and sand. I suppose I am asking a lot of the OG z carrage + a downcut sprial and 1.5" stock but still… sucks.

All-in-all the jig is a better option and probably a timesaver at this point.


I had dealt with tapering of locating holes in hard material. Make sure to do a test cut and check for issues. Ahh ok nm too late haha.

Chuckle, just a bit.


@neilferreri if you do decide to do the CNC route make sure that you use a finishing pass or stock to leave and then a finishing pass. I’m finding that from the UNDERSIDE of the 1.5” birch my 20.2mm dogs work only with the holes that I had the shapeoko repeat for one reason or another. The TOPSIDE is a-okay but the bottoms of the holes are too tight. Probably similar to the tapering that @BubbyDog mentioned


Looks great so far Mark, don’t want to jinx you ha ha.
Different materials take different size holes to get the results I wanted on my XXL. Holes in soft material taper much less then hard.
I got my best results on locating pins in 1/2" 6061 Aluminum with a .005 doc contour and 30,000 rpm. Still have taper but I could get my pins through the bottom which was the only part of the hole that is not tapered, accurate after cutting a series test holes to get it so my stainless locating pins can slide in with slight effort and no side to side play.
I cut my 1/4" holes in .5" aluminum with a 1/8 single flute and used a .2615" hole in fusion.
For MDF I had to use a smaller then 1/4" hole, used a 1/8 downcutting 3 flute. My 1/4" hole size in fusion was .2375" @18000 rpm with a .1 doc contour. end result is much less taper.
Hardwoods varied but were slightly smaller hole then Aluminum, with around a .255".
For any pinned operations, I make a series of test holes in each material before starting, to get my pin size measurements exact before proceeding with actual stock.
Note that different thicknesses cause different amounts of taper. A 3/8" piece of aluminum would need a completely different size hole then 1/2" plate will.


All done. If anyone wants to duplicate the toolpaths in step7 and step 8 of my setup I found to be the best. The second half turned out as perfect as i have tools to measure for across the full length.


The issue of being out of square is to fold. One difference in temp and humidity makes the wood move, and 2 if tou dont tram and have everythimg on the s3 perfectly square, it will be off in distance.
That could be why tight in bottom of the hole, rhe z may not be perfectly square.