I am making a new table for my drill press. I want to cut out a half moon shape on the back edge to go around the drill press column. My drill press table is 2 pieces of 19mm Baltic birch glued together for a total thickness of roughly 1-1/2ā. My 1/4ā router bit has a cutting length of 1ā. I think it will be okay, since I am only using about the bottom 1/8ā of the bit to actually cut, but I would like another opinion.
When I do cuts on thick workpieces, Iāve realized the stress levels go to zero when I do the last bit with a jigsaw. I just flush trim after that.
2 Likes
Iām with @NeilFerreri . I have the luxury of a band saw and a router table. In your situation, I would leave the 1/2" uncut by the CNC, then cut it offsized with my bandsaw, and finally use a flush trim bit in my router table.
If you donāt have those machines, you can chance it, cut from both sides, or buy an extra length 1/4" end mill.
1 Like
Is there a reason to not cut beyond the fluted part of an end mill if the shaft is the same diameter? I āassumedā it was okay as long as I still had the shaft in far enough to reach the top of the collet and I wasnāt just drilling a hole so the chips had a way to get out.
Like I said this was just because I didnāt see anything wrong with it but Iāve been wrong plenty of times beforeā¦
@_Michael There are two schools of thought on this, apparently. In fact, there is a recent thread on the Vectric forum about this very thing.
In short, I believe that, as long as the shank and the flutes are the same diameter, there is no issue. I guess thatās obvious. Apparently, though, there are bits where the flute diameter and the shank diameter are not quite the same. In these cases, you can get burning. Another issue is that, with small diameter bits, you can get flex when cutting beyond the flute depth, which can also cause burning - amongst other issues.
1 Like
Well, I chose the safe route as suggested and only cut 1ā deep. The part I am making is 18 x 30 inches, so it would not fit on my band saw, so I cut the rest of the way with a jig saw. Again, because it is so big and heavy, I had reservations about trying to slide it into a flush trim bit on my router table, so I used my trim router and finished it that way. All done and it fits on the drill press. Thanks for all the help.
2 Likes
Usual preface, Iām with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
Short version is that itās always an issue even if the cutter diameter is the shank diameter. This is because other than tools with land (unground section behind the flute) you lose part of the diameter of the shank to make flute and relief of the cutting tool. This is why youāll see a different spec when listed for diameter tolerances on tool the same diameter as the shank. This means that any tool that is listed as the same cutting diameter as shank size is actually slightly smaller. Even if you could perfectly grind it the initial wear would make the flutes slightly smaller. Add in runout and now you are rubbing the shank even more.
The above is separate as to if you can get away with it. If you can cut fast enough and have a rigid enough machine you CAN get away with it. To be clear I wouldnāt recommend it and you would need to adjust feed/speeds and babysit it the whole time.
Thereās still 2 other issues you have, the first being stickout. Stickout (the amount of tool āsticking outā of the collet) does not just make small diameters more likely to deflect (bend). A quick example would be in a generic carbide/geometry 1/4" diameter, 1" cutting length tool it would take about 12.3lbs of force to deflect the tool 0.001" with 1.2" of stickout. If with the same tool we leave 1.7" out of the collet (stickout) it only takes 6.8lbs to bend the tool the same amount (pulled the numbers from Millalyzer).
The final issue that Iāll go over is the collet engagement. You need to have enough shank left to seat in the collet. Din standard is 4x the diameter or length of the collet for non-ER collet I would just default to the length of the collet. So you need to have at least that much left to insert into the collet or risk poor clamping and/or damage to the collet.
Hope thatās useful. Let me know if thereās something I can help with.
4 Likes
I was wondering if you would chime in when I was asking my question. As always you provided some good information that makes sense to me.
I imagine that there are a bunch of things that I can get away with, not that I should, because Iām working with wood.
Thanks again!
No problem. If thereās ever something you or anyone else want me to address feel free to @ or PM me. I donāt always get time to go through the posts.
2 Likes
Very good information, thank you for posting. I guess Iām glad I asked the question, I have learned a lot.
I have just been going through this cutting pieces up to 2" thick. My solution was to use an appropriate bit for the task. Spetool make a 1/4" shaft extra long bit (SpeTool Spiral Router Bits with UpCut 4 inch Extra Long1/4 inch Cutting Diameter 2 inch Cutting Length CNC Router Bit Carving Tool : Amazon.ca: Tools & Home Improvement ) with 2" of cutting length and 2" of shaft length. It happens to be on Black Friday sale right now at a great price. I dialed down the typical stepdown and travel speed by 50% having consideration for the stress on such a long bit. I have used it several times now and it is still in one piece. Some of the Amazon reviews say that it broke when first used, and I guess that is possible considering the length of the bit . Perhaps they were being too aggressive with the cut parameters.
2 Likes
I saw that bit on Amazon before I started this thread. I even measured to see if it would fit. It just seemed too spindly and breakable. Glad it is working for you, I may consider it in the future.
I had the same concerns but āslow and steady wins the raceā. You were right to be skeptical. My alternative was to cut 2 pieces and glue them together, which would not have had the same good appearance in my case. Patience is a virtue, and for woodworkers it is very often the difference between success and failure. We are all eager, sometimes to eager, to get a result. Anyone who hasnāt broken a few bits either through ignorance, or poor prep has either been beyond lucky or hasnāt done very much.
1 Like
In your software, add two 1/4" holes into your design. Set the XY zero to the center of your design. The second hole should be a mirror of the first along the X axis.
(an equal distance from the center Y axis) just inside the outline.
Using your cnc drill the two holes into your spoil board using a 1/8" up-cut end mill. (3/8" deep should be good.)
NOTE: Donāt change the XY setting in gsender.
Using blue tape and CA glue, mount your raw stock over the holes and repeat the drilling of the two holes into the bottom of your stock.
Remove your stock, add dowel pins, flip and mount your stock with blue tape and CA glue.
Again drill the two holes in the top of your stock.
Cut your outline to >60% of height.
Remove your stock, move dowel pins to the top, flip horizontally and mount your stock with blue tape and CA glue.
Cut your outline to >60% of height.
I hope I have said this correctly.
I had good luck using this method to cut two sided designs (bowls, etc)
Good luck.
1 Like
I have seen this method for 2 sided parts before, although I have never used it. In this case, I was making a drill press table and drilling holes in the top surface was not an option.