View Full Version : Question about two sided machining article
04-16-2009, 09:57 PM
So, I'm reading my digital machinist magazine article "indexing for two sided machining" on page 52 spring 2009. If you don't have a copy yet, or don't subscribe, my very poor summary of a well written article with good pictures, is the author machined all sides by drilling locating holes in the stock outside the perimeter of the finished product and then when flipping the stock to get the other side, he pinned the stock thru the locating holes into a solidly anchored bar of MDF (MDF = partially synthetic composite wood material)
Why not, when machining the first side, carve both a vertical and horizontal channel completely thru the raw stock, with the inside edge at some precise and known offset from some known point on the product, into a semi-sacrificial "fixture" underneath? After side one is done, flip the stock over and pick up the X and Y using my handy dandy edge finder. My edge finder can more accurately locate X and Y off a nice long machined edge than using pins in wood?
Now as a disclaimer, I'm not trying to pick on the article or author because:
1) I'm a total newbie and I'm not trying to be the new guy with all the answers, but genuinely asking why not my idea?
2) Success defines its own truth, and since what the author did worked, then his way was one good way to do it. Does my way work too?
3) Closely related to #2 above, I fully acknowledge a large gap between my "I think this might work" and his "That worked when I did it".
04-17-2009, 08:17 PM
If I understand correctly (I haven't seen the article) both ways work. I too would be concerned about MDF holding up but for an one-off it's probably okay. My biggest hangup would be that it sounds like both methods are wasting lots of material. If there is a lot of profiling to do and the waste areas for the pins/locating feature are part of a logical blank than they are great methods. If you are using a really oversize blank just to have somewhere to locate it sounds wasteful. For multiple parts, his method would better in that it is faster. Just flip it over and the pins locate the part without having to find part zero for every piece.
I like to use homemade aluminum sub plates/ fixturing blocks. If the part has holes, I will drill & ream them under their final size in a slightly oversize blank and use some to locate with dowels and others are used to bolt the piece down. Your blocks will soon look like swiss cheese. Or if the hole location isn't supercritical (IE, clearance holes for bolts) I will drill them right at nominal for the holddown bolts and locate off the bolts to do the profiling of the part. Afterward they get opened up to their final sizes.
I have a couple of nice aluminum sub plates that I have put in a grid pattern of tapped and reamed dowel pin holes. I will push the part into the dowel pins to locate the part. Once its clamped up, I can pin punch the dowels below the surface of the sub plate to allow access to the part.
With these I often have to switch the clamps in the middle of the program to get at all areas.
Sometimes I will machine into the fixture block slightly to get a clean edge on the part. With fixture blocks that have some effort in them nd I don't want to use them up too fast I will stay .010" off the block. The thin lip on the part can be broken off with pliers and cleaned up with a file.
The most common method you will see is to use a overly thick blank and leave enough above the vise jaws to do all five sides and then flip it over and face mill to the final thickness.
There are lots of clever methods to avoid having to combine squaring up a blank with all the other operations. I hope this all made sense and sorry if I rambled but clever fixturing and programming is the fun part of machining for me.
04-17-2009, 09:02 PM
Just realized for your method how are you aligning the workpiece to the machine. If you are using a vise, all the finished edges are still in a rough blank if I understand correctly. I am visualizing material left all the way around the workpiece with no exposed finished edges. You can find the location of the slot but the finished piece isn't necessarily square with the machine. If you clamped it to a plate you would have to run a test indicator along one of your slots to align it. With the articles method the pins locate and align it.
In the methods I talked of, the finished sides of the workpiece are exposed so when its flipped over it can be located for the work zero AND square with the machine.
04-17-2009, 10:34 PM
I'll agree with what the monkey said.
There are a million ways to flip and locate. First off I would disregard the MDF and think solely about the technique, not the material. I only like to use wood for welding fixtures where it can go up in flames.
On the using an edge finder, why? say you are doing 10 parts or 1000 parts or even 2 parts. Flip and hit the green button or screw around with an edgefinder for each part and set a new offset. I'm all for flip and go.
Alternately if you need to flip 90 degrees up onto an angle plate, the dowel pin method is pretty darn handy, weather sacrificial or tightening up the tolerance on existing holes.
Vince to answer your questions.
1, 2 and 3) Too slow for multiples or when you simply can't get to a machined edge when flipped, or in your case, can't chew in some channels, but you are definitely on the right track with the thought process, thats a good thing and I have used existing channels/slots in a part to locate it on the flip side. Also, when you don't have the thickness to add channels and/or an irregular shaped part that isn't going to lend itself to two machined edges square to each other. Also, drills and reamers are cheaper than endmills.