I have been trying to CNC a dog hole template following MFT dimensions, i.e. 20mm holes 96mm on center. I am consistently getting undersized holes by about 0.4 mm (holes are 19.6mm) which is a problem since dog holes are machined to at least 19.95mm.
I am using a Shapeoko 5 pro, with a C3D #201 bit and a bore toolpath with a stock to leave of 0.2mm, followed by a second bore operation (finish) with the same cutter and with finishing and spring passes enabled. The finish bore op is running at 18,000 RPM with a cutting feedrate of 1230mm/min. I am doing the tests in baltic birch 3/4" plywood.
There are no belts in the Shapeoko 5 pro, but I am tempted to run the v-bit pricking test to see if there’s anything off in the steps/mm unless someone else has a better idea about what could be going on. Any guidance / help to debug and correct this would be nice.
There will be others who do more precision work than I usually do, but some things to check in addition to the steps calibration are:
Deflection- if you are doing dogholes, I assume the cut is very deep and probably in a hardwood. Do you have the bit sticking out more than usual, and pushing the cut speed? The higher loads can deflect the bit. One approach is run a second pass, the loads would be much lower on the second pass and there won’t be much deflection.
Undersized bit-An error in the diameter of a hole of 0.04 mm, could come about with a bit that is 0.02 mm undersize, that is less than a thousandth of an inch in imperial units. Is it a new bit or well used. (to be honest I have no idea about how much the diameter changes on wear)
The high precision folks will probably chime in with some other suggestions (possibly while I write this ) But figured you are in the middle of a big project on a holiday weekend when you have time
John
Edit – realized on Adrian’s reply I was off by a factor of 10 when remembering his error amount. (Is there a way to have the post you are replying to visible while you write the response?
Above should be 0.4 mm not 0.04 mm. Still that is about 8 thousandths of an inch off (0.2 mm)
Sometimes bits just aren’t quite as precise in their dimeter as spec’d - I would check the bit with a good pair of calipers. Additionally, check for any slight play in the Z-axis or dead-space in the X/Y axis ballscrew - I believe some people have found a slightly loose mechanical connection with the motor couplers.
Writing that prior reply got me curious (and gave me an excuse to step away from preparing for next week’s classes I am teaching). I ran out to the garage and measured both my 201 I have been using for some time (thought I mainly reach for Cadence MFG “Jenny” bits now), and an unused 201 I bought as a backup bit. Both bits were a little undersized measured by a Mituyo caliper. This is with the caveat that bit diameter is pretty challenging to measure accurately.
I suspected this, and the way I measured was to run a straight cut using the MDI with the #201 and measuring its width. I got a 6.22mm instead of the advertised 6.35mm. So while that could explain part of the 0.4mm gap, it doesn’t account for all of it. Bits are sold for machines that are much more precise than Shapeoko though, so I expected them to be almost dead on? I would hate to have to run a test cut for every new bit and adjust its description in my CAM’s tool library. Is that what people do?
I can run a test by setting the bit diam in CAM to the actual 6.22mm I measured and see how far off it is. It should be 0.14 off (i.e. 19.86mm) which is much closer but still would not let those dogs in.
Did you run the job twice?
I just cut holes for a .250 dowel pin in cherry and MDF.
I had to add .004 to the hole.
It was still too snug, until I ran it the second time.
Now it a snug slip fit.
Both were effectely blind holes.
I run the same operation twice, with spring passes and finishing passes, so there should be no deflection. I also have tried this twice with different feedrates as well.
You will find almost everything produced/machined has “instrument error in-accuracies”. We operated for years with analog gages and were happy to record to half the marked value/increment on a gage. Later came digital recorders and indicators that read out to the hundreds & thousands even tho the system was running the exact same parameters, we could just “see” that much finer detail.
I use a 0.25” bit, program the toolpath to set a 0.75” dowel into it. Sometimes it fits, sometimes it don’t. The dowels are not uniformly 0.75” down its length, the wood/mdf after the cut pulls in moisture etc.
I get as close as I can and if I have to I will tweak the toolpath to make it fit, not ideal but it gets the job done.
I work with machinist and we do a lot of iso projects.
It is very important to take precise measurements of your tooling. On your dog holes measure your bit, check to make sure your spindle is squared to the table front to back and side to side. On bit defection do a 1mm inset on each hole use this inset line to cut a climb cut to remove the bulk material. Then create a conventional cut on the original hole size. Make sure you have done the math on your chip load. Old guys at the shop do it by ear and the rest of us young whippersnappers use FsWizard app.
I looked up FSWizard and saw comments that HSMAdvisor had more accurate data and certain plans included FSWizard Pro. Any feedback on HSMAdvisor or FSWizard Pro accuracy and value?
Im having a similar issue. Earlier today i was making a bit holder for storage. I measured the case for a 1/2" bit which was .70. I oversized it to .72 to give wiggle room and the case fit fine. I then measured for the 1/4" case at .5" and oversized to .52. The result sucked, so i kept oversizing and at .64 the case fits just as it should. Ill be talking to carbide tomorrow to see whats going on.
Curious to hear what you find out. After checking the steps/mm, and adjusting speeds & feeds and CAM as much as possible I had to set a negative stock to leave of 0.08 to make it work.
Well, it wasnt the machine in my case…newbie still. I did a test today and got the same result on the sizing. I clued in that i didnt have my tool dimensions set properly, i set the shank size at 1/4" and the cutter is 1/8". Once i changed that it was a perfect cut.
) But figured you are in the middle of a big project on a holiday weekend when you have time