Proper toolpaths / configuration for cutting holes in an MFT table top by CNC

[MaximeLesveque]

I went to a local CNC shop (the only one in my area) and asked for a grid of 8x14 holes of 20mm diameter, and figured it would be a trivial project.

Having read a few discussions on the subject, I asked that they do a few tests first, and gave them a bench dog that is machined at 19.99mm for testing (made by BenchDogshttps://benchdogs.co.uk/).

They came back saying that they had to make holes of 20.4216mm in order to be able to insert the dog. The diameter of 20.4216 was obtained by trial and error, with after 2 attempts.

When I inserted the dog in the 20.4216 hole, there was no play at first, it had to be really forced in, but after a few insert and removal, there was significant play, while inserting, and the play ends only when the dog is completely inserted, as if the top and bottom ring of the cylindric hole had a tighter/smaller diameter than towards the center.

Question: are the holes in the original festool table actualy 20mm ?

I noticed that Seneca Wood Working has a CAD plan with 20.2 mm holes, and I read a few discussions recommending enlarging holes a bit.

Also, the tests have been made on 18mm baltic birch plywood, and not HDF (it seems that HDF is impossible to get in my area, and apparently MDF is not not great, so I was intending to go with baltic birch ply).

Does baltic birch ply require larger holes given that it's density is less evenly distributed than HDF ?

I also didn't ask them to chamfer the holes prior to testing the fit. 

Could be that just chamfering could be sufficient to getting an exact 20mm would work ?

Or perhaps, given that I'm using ply instead of HDF, I will have to settle with 20.X hole, even with a chamfer, hopefuly X smaller than 0.4216 !

The CNC shop uses VCarve, the machine seems quite decent, it would be great if anyone could share a VCarve configuration that is known to work, I realize that there are many cutting and toolpath configurations, and not all of them are good.

I've read things about first making a rough cut of 19.9mm, followed by a finish cut at 20.mmm, using, spiral cut paths, etc, but it would be so much simpler to give a vcarve file !

Thanks !

 

[tsmi243]

I don't have a specific answer to your problem, but will agree that Baltic and MDF will not have the same "fuzz" inside the hole, so you really should test with your final material.

I also can't say why, but will say from experience that a chamfer CAN significantly affect the feel of the fit.  So definitely try that before finalizing the diameter.

Also check here- AtomicRyan had his top CNC cut, and they had some consistency issues.  So you may not be able to count on CNC alone for accuracyhttps://www.festoolownersgroup.com/festool-jigs-tool-enhancements/bfmft-build/

 

[infer]

I have used my laser cutter and cnc machine to make various jigs for benchdogs. 19.9mm is the correct hole diameter. Maybe they are not imputing the correct bit diameter to the CAM software!?
Nice tight repeatable holes on mdf. On first insertion very tight but loosen a bit after use.

 

[Oldwood]

I found the solution was to get a drill bit for the CNC that cuts the size of hole you need. Most of the 20 mm carbide boring bits will give good results.

If you have a very accurate caliper or micrometer, you can take it to the store and check the diameter of the bits.

Routing out the hole is never going to give you the repeatable result that boring will with the right size of bit.

 

[GigaWatt]

I've owned a CNC for 5 years and cut 3 MFT tops for myself and several for other people. You need to check the actual diameter of cutters when you buy them. For example a 1/4" end mill I'm currently using measures .247" diameter and you need to compensate for that difference in the software for an accurate cut dimension. I've tried both BB and MDF, prefer MDF.

 

[MikeGE]

For example a 1/4" end mill I'm currently using measures .497" and you need to compensate for that difference in the software for an accurate cut dimension.

[eek]  Am I reading this correctly?  Is the .497" the length of the end mill or the diameter?

 

[GigaWatt]

For example a 1/4" end mill I'm currently using measures .497" and you need to compensate for that difference in the software for an accurate cut dimension.

[eek]  Am I reading this correctly?  Is the .497" the length of the end mill or the diameter?

Sorry, don't know what I was thinking, it should be .247" dia. I corrected OP.

 

[MikeGE]

Sorry, don't know what I was thinking, it should be .247" dia. I corrected OP.

[big grin]

 

[savsuds]

Thanks for the info MikeGE. I played around recently on my CNC to dial in the right diameter holes to fit my TSO tight fit dogs on my Shapeoko Pro XXL. I should also measure the bit’s true diameter if the current one becomes dull or breaks. I forget that not all bits are the published size when they are used for a CNC router.

 

[afish]

I have ran a couple full 4 x 8 tops in MDF and after a little trial and error I found 20.2946 to be the best fit for the veritas dogs that I had.  However just because my machine/dog combo likes 20.2946 best doesnt mean that is the magic number for others.  There are a lot of variables that can effect cnc cutting performance as some here have found out.  Not only does the CNC machine itself vary but the person who sets up and tunes the CNC is just as important as the machine itself. You can get worse cuts from a 100k cnc with someone who doesnt know what they are doing than a 20k machine with a good operator and tune.  People who dont own and operate CNC machines sometimes have a misconception that its a CNC and .001 on one machine is .001 on all or its automatically perfect.  In theory yes but in real world NO. 

Every CNC has a certain amount of "backlash" Backlash is the amount of distance lost when the cnc changes direction all machines have some backlash (some have very little .001-.002 and I have seen some in excess of .020) point is all have some and its different from machine to machine depending on numerous factors.  You can adjust the software to compensate for backlash but now you are counting on the operator to measure and adjust properly.  Which takes time plus trial and error making test cuts. 

As someone else pointed out "true" cutter size is another factor and an even bigger problem if using re-sharpened cutters.  Its very easy to get a large collection of bits after awhile and loose track of whats what.  Getting a accurate measurement down to .001 on a spiral cutter isnt the easiest thing to do either.  Even the cut speed and cutter diameter will come into play a smaller diameter bit will flex more and the faster you push the cutter the more bending force you will exert on the cutter.  If you try to push to far the machine can also lose position or steps if the CNC has stepper motors.

How square the cutter is to the table is another common source of error.  The cutter needs to square in both the X an Y axis if its off in either or both it will cause issues.  It needs to be trammed for best results. you cant simply put a square next to a cutter like you would check a table saw, at least not for best results. 

Another variable factor in setup is adjusting the length of cut depending on the transmission of the machine which is usually Rack and pinion for the X and Y and ball screw for the Z you have to set up the software and adjust so .0xx" in the software matches .0xx" on the machine.  Simple right? not so fast.  It gets difficult and expensive to measure large distances down to the thousandth. Its also more accurate to measure over a long distance than a short one.  For example when I was setting up my machine the first time I used a 6" dial caliper to measure some test squares but when I started making long cuts I noticed I had more error.  So I ended up using a tape measure and a small V bit as an indicator and adjusted based off the full travel on on the longest axis.  This gave me the best results for large items and Im usually under .003" error on small stuff that I can measure with a caliper.

This is just a short list of some of the common items that will effect the precision of CNC cutting. Long story short just because its cut on a CNC doesn't mean its going to be perfect. Circles and ellipses are notoriously hard for a CNC to get "perfect"  When you have a machine trying to move a cutter in 2 different directions that needs to change and adjust the position 100's of times per second there will be plenty of possibilities of error. not to mention the human factor.  Even the best machines can and will have small repeatability error of a few thousands even when cutting the same part on the same machine.  So its important to have a reasonable expectation of what's perfect or acceptable. At the end of the day even if some how by the grace of god you got lucky enough to get hundreds of small holes perfectly square in a 3 axis pattern with every hole precisely at 32mm spacing down to .001" its wood and is subject to movement based on temp and humidity.

Anyone that is concerned over several thousands will never be happy cutting with dogs (period) If you want the squarest and most accurate cuts you will need a MFT with a fence and rail hinge (NOT THE FESTOOL ONE) type cutting station and leave the dog holes for clamping and fixturing. It doesn't matter what you are cutting with, a track saw or 100k plus cnc you will always be chasing perfect.