Is there any way to bore a ≈1in deep 4.917mm diameter hole with an endmill? I can’t find any 3/16 or 1.8 endmills with a 1in LOC, which makes sense because of deflection.
Having a fixture plate thinner than 1 inch from the frame would mean that I wouldn’t be able to reach the bottom with some endmills.
Alternatively, I could use a #10 (4.913mm diameter) carbide drill only and hope that i’ll land somewhere close to 4.917, then thread mill. Would that affect the actual thread by much as compared to boring?
It would be simpler to just machine slats out of HDPE and mount a 1/2 fixture plate on top, but then it would require squaring with a dial indicator every time I take it off.
Several things. If you want to get a reasonably accurate hole and not have to worry about chip clearing you will want to drill it with an undersized drill bit and then bore it to size with an end mill followed by threadmilling or manually tapping it with some sort of tap guide. To reach the full depth you can do the bore in 2 steps. First bore to the max depth you can with your tool, then bore the rest with 0.002-0.003" stock to leave. This only works if the shank of your tool is not any bigger than the cutting section. Here is something from Harvey Tool that has the reach required with a relieved shank though you will need to be careful about clogging it with chips. Drilling through first so the chips can fall out the bottom and following the advice from this youtube video will help:
Also, if you are worried about being accurate enough that you are measuring with an indicator, you will probably need to use an indicator every time you remove and replace your fixture plate regardless of whether there is HDPE involved.
Thanks for the advice, I was mainly looking at single flute endmills but I think a 3 flute with airblast should work too given that it’ll only be finishing passes. I think either that or I can set up an MDF fixture with a recessed box that allows me to flip the fixture plate and bore the underside with a shorter endmill but I’d rather not introduce more opportunities for user error.
As for squaring the fixture plate, if I directly mount a full coverage plate to the frame, I can square it once and attach a full-sized wasteboard on top when needed, vs having a detachable smaller fixture plate mounted to the T tracks that I would have to take off to mount a mdf wasteboard
For clarification, with this 5/32 1.25in reach endmill: Harvey
I bore the hole to it’s exact size to the depth of the maximum length of cut, 0.234in, and then bore the entire depth of 1 inch but with stock to leave. Wouldn’t cutting below the flute length cause problems with rubbing or does the stock to leave offset that? How would a finishing pass work?
Sorry if I’m asking a lot of questions, I’m still relatively new to machining aluminum
Pretty sure that tool you linked has a relieved shank meaning that the cutting flutes have a larger diameter than the neck of the tool. You would not need to do multiple steps using stock to leave. That method is only for cases where you don’t have a relieved shank. This is the case for the tool I linked to as well.
Did you end up facing the entire thing afterwards? I don’t know if the HDM can get ±0.005 across the entire cutting area
Griff
(Well crap, my hypometric precursor device is blown…)
43
I did not. I faced each plate individually. I will do so on my next attempt. That will be a plate limited to the cutting area of the machine, 7/8” or 1” thick, mounted on the frame.
I’ve learned that covering the entire HDM surface with fixture plate is aesthetically pleasing but not particularly useful. At least for my needs.
Fwiw, I did use the non cuttable area of my 4 Pro fixture plates when I was running a set tiling jobs on pieces 30" wide and 32-48" long. Using the extra space gave me extra material for clamping while still using almost my full cutting area for the project.
So, there is very occasionally a use for it but it’s not going to be often…
Will I be needing a spot drill to drill 4mm holes at 1in deep? I think there would definitely be deflection from the long carbide drill bit but considering that its only supposed to be an opening for the boring operaition, would I need to spot drill it? I’d rather not have to get an extra tool and a couple hundred more operations. Thanks
I read at the article but was somewhat unsure. I have a 4mm carbide drill, but it’s also a jobber drill, (80mm long). I think I should be fine but I wanted to make sure.
Since you have a HDM, you could probably get away with it. As for myself, I have a Pro 4, and as it’s a rubber band drive, I would spot drill them all first, and then come back with the 4mm jobber’s bit. However, in the eleven hours since your post, they could have all been spotted and drilled.
Griff
(Well crap, my hypometric precursor device is blown…)
49
Following your thread with interest. As I consider my new design.
I picked up a Datron single flute, 5mm x 22mm doc. I prefer the F360 bore toolpath to drilling. So, 20mm thickness for my final plate, 6mm hardware, carried over from my first plates.
1 Like
Griff
(Well crap, my hypometric precursor device is blown…)
50
This test piece is set up for inserts rather than 6mm threaded holes but the basic design applies to both.
The center section, the actual fixture plate, is 26” X 20” (slightly smaller than actual cut area). This provides wiggle room for machining/facing. It sits proud of the side and back plates a few millimeters. Also, if need be, the sides and back can be removed and shaved down to enable deeper re-facing of the fp, an important feature for me as I make a lot of mistakes!
I’ll stick with the mdf sides and back, at least to begin with and machine the fp from 7/8” ATP5.
How are you progressing?
What I found on my non-surfaced MDF fp:
About .0015” in X and about 0.004” in Y. Kind of surprising I think.
