does anyone know how these things are made or how i can find something like it.
You could mill this but it would take a lot of tool changes and 5 different setups (top and one for each side).
If it doesn’t have to metal you could also print it, though if any hole sizes are critical you will would likely need to redrill them after a print.
1 Like
Or simplify the design if certain details aren’t so important. Depending how large this is, those internal corner cylindrical channels look especially challenging to mill with how long and narrow they are.
There is alot of wasted material if you mill this, i would find a way to save some material by hand cutting those large chunks (almost entirely that way you dont screw up by accident) out then let the mill precision cut everything, it saves you alot of time and material can be recycled easier this way.
2 important questions:
- What material?
- How many?
If you’re making 1 a hog out is the only practical way to make it quickly. Also if you need a good surface finish.
If it’s the right material and you have connections you can print it but the post processing may drive the cost as high or higher than milling. Especially if the material and properties require HIP
1 Like
There are many, many ways to make most widgets. But there isn’t enough info provided to give a more accurate answer. What is it made out of? How big is it? What are the tolerances? What is the surface finish? What is the quantity? What is the budget? Anything else “special” about this part?
Answering most of the above would help determine the most efficient way to make it.
If this is a single/few fictional part, and assuming it’s laptop-ish size, I’d make it on a milling machine as other have said. Several setup and tool changes.
If I had a machining center with a rotary tombstone, it could be two setups; one to face the top, machine the big square hole. The other to make the features on the four sides with a rotary indexer and tombstone type of mounting.
If it were a gazillion pieces out of plastic -injection mold.
If it were hardend tool steel -EDM
If it were thousands out of aluminum, -dedicated fixturing
If it were a weldment -well, I guess it depends where the welds can be located.
If this were the size of a house -IDK, I don’t build houses, but it would involve other techniques and “layering” of those techniques.
You get the idea.
re: internal corner cylindrical channels look especially challenging to mill
I’d guess it’s clearance for a sharp corner thing that fits in the square. Regardless, I’d drill the four corner before cutting the sqare.
2 Likes
Looks like a bearing block for a tube in tube telescoping assembly. So I’d maybe 3D print that, or go way simpler and just machine a Delrin slider block
1 Like
Your question implies that it’s not something that you guys designed in CAD, but is, instead, something you imported from elsewhere. Where did you find it?
And, how big is it? What’s the height?
If you guys designed it yourself, a number of those holes are very close to the edges, so those holes are not going to be very strong.
First preference: I wouldn’t. If a student came to me with this design I’d tell them “no” and we’d go to the whiteboard, back up a step, and find a way to tweak the design to not require it.
Second preference: If the design truly couldn’t work without this and we were too late to pivot, I’d turn this into 4 simpler parts and bolt them together, maybe with some pins and slots to index them together. It would be cheaper, easier, (probably) faster, and lower risk.
Third preference: If we were somehow backed into a corner where the only option were to manufacture this part: It would require at least 5 setups in the mill. I’m not an expert machinist, but I could probably step-by-step my way through it.
- Get a piece of stock that’s oversized a little in X and Y and a bit more in Z (height).
- Square the stock and take the X and Y to final dimension.
- Drill/mill/bore the holes and slots on the smaller sides, always indexing off of the same sides and edges to try to control my tolerances.
- Clamp up with the bottom edge of the block supported by the top edge of the vice for the last big material removal op.
- Drill the inside corner reliefs.
- Rough out most of the stock with a large end mill, leaving just a few thou where possible.
- Finish the material removal with a smaller end mill.
- Flip the part and flywheel off the remaining material on the bottom.
Always reduce your stickout on both the part from the workholding (vice) and your tool from your tool holder, always keep track of your zeros, and always check your feeds and speeds.
(The IRL answer is that I’d make it @Skuke and @RoboChair’s problem and come back a day or two later when it’s done 
)
9 Likes
I agree with @BordomBeThyName on “just no”
But if I had to machine it… I’d modify it so the slots for bearings went to the top and bottom surface so I could do it in 2 setups (top and bottom) and then print a drill guide block and do the side holes on a drill press.
The what I assume is a bearing hole, I’d remove it entirely, make it clearance for the shaft and then make a block that filled that space so I could skip that hole.
Try 1 would be print it though.
2 Likes
Echoing the above
- don’t. Time for a redesign or go to COTS. If it has to be metal try to make it out of two parallel plates joined by fasteners. Otherwise see point 2.
- 3d print with design alterations to remove unnecessary/minimally useful features and beef up what matters.
- If there is no way around it: simplify, try to get it out of two plates, reduce any features that aren’t holes, try to get it made in 2-3 set ups on a mill max.
(Substantial Language warning)
5 Likes
CLASSIC video. Absolute must-watch for anyone [that the language is not an issue for].
This topic was automatically closed 365 days after the last reply. New replies are no longer allowed.