Is milling your own fixture plates worth it?

My guess would be for shipping. They have larger plates for other machines, but I’d wager they get shipped freight instead of parcel. I worked for UPS and did shipping for a company that made larger car parts. Shipping gets experientially more expensive with size once you get past a certain size. Also the package is more likely to get banged up the larger and heavier it gets.

It could also be that they run hobby machine size plates on a certain machine and industrial sized plates on larger machines.

1 Like

I spent some more time designing, considering that I’m making them custom, I’m thinking about mixing in some 1/2 threads for use with more work holding options. I could alternatively just use 1/2 and mount a m6 plate on top, but thats a lot more aluminum.

Considering that the HDM is a pretty powerful machine, I feel like using only M6 would be a bit of a waste. Thoughts?

I’m not sure the M6 is going to be the limiting factor. The clamping forces from bolts are surprisingly large.

Is an example, it’s for all steel, not steel & aluminium but still, 500lbs clamping force per bolt for M6. So long as you make reasonably good, deep threads to spread the load through the Aluminium plate, something else should be the limiting factor.

7 Likes

Can anyone recommend a 4mm or 5/32 drill bit? I’m not sure if the ones I found would be appropriate for the HDM’s spindle speeds.
I ran a M6 design through fusion 360 and it would take quite a lot of time to bore out each hole.

Also do I need to have mist lubrication for drilling? I have airblast set up and am working on a mister, but I’m going to be using a MDF wasteboard and I’m worried that the extended moisture exposure would cause it to warp.

Assuming you’re in the US, PreciseBits is worth a look, they have some high speed carbide drills

A follow up boring op of slightly larger diameter would give a well defined hole for locating pins or tapping.

I would suggest lubrication for drilling, I’ve used a syringe to squirt Isopropanol for drilling 6083 Aluminium, an air blast with coolant mist would likely be better.

As for the wasteboard, given the cost of the Aluminium I’d suggest a sacrificial additional board which you mill level if you don’t want to damage the spoilboard on the machine, Isopropanol is very good at evaporating away before it can damage the MDF though.

1 Like

Does anyone know if there’s a set of S5P plates coming? The older ones aren’t compatible with the 5!

The 12x12 plates from SMW should be compatible with the 5 as long as the T Track widths are spaced the same as the 4 and HDM, which I’m pretty sure it is.

They are not as noted in the announcement:

https://carbide3d.com/blog/introducing-shapeoko-5-pro/

The table T-slot spacing is now 4.04”, instead of 100mm.

Here is a reply about asking if they were doing something for the 5 specifically which I received on the 14th.

“Yes, we are working on a plate design and are hoping to have more info available in a few weeks. I’ve got you on our waiting list so we should be reaching out soon!”

1 Like

They being SMW….(20 char)

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:

https://www.harveytool.com/products/tool-details-937112

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.

2 Likes

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

Interesting about mill threading! Never seen that before. Are folks doing that on their shapeoko machines with success?

Yes, folks have done this:

2 Likes

Here’s a clip of thread milling a section of fixture plate.

If I figured it out anyone can.

8 Likes

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.

1 Like

Ah ok, I thought relieved shank meant the difference between the neck diameter and the actual shank.