Question on How To Cut Part

[Hellbringer]

Hi,
I am working on a project that have to cut 145 of this part:



there are 4 features to the link (2 holes on top, 2 holes on side, stagger, and arc on on side) and as far as i can see i can only cut 2 of the 4 with any position that i put it on the mill so i would have to flip the stock to be be able to cut the other 2 featues (so if i put it top up i an cut the stagger and the 2 holes on top, but i cant cut the 2 holes on side or arc) right now the only way i see to do it would be to cut one of the sides (2 features) and then cut the other 2 features on each and every link and with 145 or so links would take for ever

is there a better way?? (besides a 5 axis mill )

also the mill is a 3 axis x2 mill with X and Y extended

thanks mike

[blades]

I think with 145 of this part, I would approach this from more of a production process aspect.

Here's how I'd do it:

1. Square up all parts, cut all sides to size

2. Line up X amount of parts (however many you can fit side-to-side in your vise. A small amount of each end piece hanging out of the vise would be ideal). Place one side against the fixed jaw, then use a folded piece of sandpaper between the parts and the moveable jaw. Then C-clamp across all the parts in the vise. Follow me so far? May want to replace the sandpaper after every few setups. The sandpaper (if not already obvious) helps to tighten down on slightly undersize pieces. The C-clamp is good insurance, and I wouldn't consider doing this type of run without both the sandpaper and the C-clamp.

3. Cut the step in one end of the parts in this setup. Repeat until all 145 parts are done on both ends.

4. Set up a work stop in the vise and drill the holes without moving the table. If the parts are symmetrical, you should be able to simply flip the part over for the other holes. At all cost, you want to avoid having to traverse the table between holes if it's a manual mill (*unless there's a very tight tolerance between the hole locations), as this will add a lot of time to the process. Keep your vise jaws and work stop clear of chips, and you should have no problems.

5. Make a fixture to drop the parts on to cut the radius on the ends. If you have a CNC, both ends could be done on 1 setup.

And that's my .02 cents worth.

[Hellbringer]

the other thing i forgot to mention ( i dont know if it makes a difference) but the parts are small the lenght is 1.05" total the holes in the side are .20"

thanks mike

[cjdavis618]

I agree with blades. but without knowing what equipment you have it will be hard to tell you.

Myself, if there are to be 145 of them, I would make out a set of fixture plates for several at a time. Are the holes on the top "through" holes or what depth? Also are they threaded?

These look like some type of link. Would this be for a track or something?

[Geof]

I will give you a different suggestion based on how we do similar parts that are small and need all the sides finished.

Do not cut out the stock for each part; cut it to a length that will fit in your machine and sufficient for several parts. You may need two vises to hold the length but this expense can be justified by the saving in time.

Also use stock that is large enough that you can grip about 1/8" or so in the two vises and machine the full perimeter all the way down for the total thickness of the part. Obviously to do this you have to have sufficient material between the parts for the cutter to pass.

Your first operation is to do the perimeter, the step and both large through holes.

Now make a very simple fixture; a long bar with a boss at each end to fit the large holes, held against the fixed jaws of the vises.

The second operation is the take the partially machined length and align it in the vises with the large holes on the bosses, and drill the small side holes.

Now cut all the parts out.

The third operation is to grip a part in each vise, face off the excess 1/8" or so that was used to grip the stock for the first operation, and do the step on that side. A stop will be needed to align the parts.

Doing it this way saves loading time because for the first two operations you are loading multiple parts.

It also saves machining time because each tool completes its operations on multiple parts before changing to the next tool. Many times the slowest operations in a program cycle are the tool changers; a lot of time can be saved by reducing the number of tool changes required.

[Hellbringer]

i understand kinda what you guys are talking about when i get home i will do a solidworks drawing to make sure

also the holes on top are not though they are about 1/8" deep

thanks mike

[Stepper Monkey]

What are the material and finish requirements like? Parts that small I would likely be lazy and investment cast to NFF, mass finish, and just hand ream the holes if I could get away with it. A lot of small linkage parts get made that way.

[KOS]

how accurate does each measurement need to be? That is my biggest question with all of this. for example is a part for an aircraft that is precision? or for a mounting point that has some play... thinking the precision needs to be close but not near perfection. Also can you buy stock that is the same width so you dont have to shave down a few thou etc...i would ask my customer if the thickness had to be .4" or if .5" would work just as well, the center "thick" area may not affect anything what so ever and only the .2" for the steps/holes may be critical....that is a massive savings in time, tooling and money right there.

anyways for 145 this is my take based on speed,

The first part I would cnc would be a flat template of the radius with the two large holes. Cut that out so you can use it as a template.

After cutting my stock to length I would then make a block to hold multiple pieces together with my template attached. If you are worried about touching your template make a couple to last, or print out your drawing and use it as a comparitor. I would then take this to my sander and get as close to those radius as possible. These can be done while you are waiting for your band saw to cut more parts unless you have some other chop saw you are using.

Move over to the drill press and knock out those two large holes with my block of blanks still intact with my template on there.

From there they would go to the mill to drill the small homes on top doing multiple blocks at a time, Unless you want to get creative with another template to use with your drill press and just use a stop.

Last step is to cut the steps out on the mill...lots more labor but they will be out the door pretty quick...your g-code for this is pretty important, this is where I would clamp down multiple parts to cut out in one run of mill, so you are not stoping to switch out a single part or waiting for tool changes all day.

If you are completely unsure, make one up like this and ask your customer if you can do a test fit to make sure you have all the right measurements from their drawing, or from yours....


I did something similar to these in the past without the steps on both sides, mine only had one. No little holes on the top either. They were just motor mounts or something along those lines and I banged them out in no time. The slowest part was waiting for the mill to work.

toss them into a vibratory tumbler and ship them out the door.

Anyways that is my .02, but like i said it all depends on the final product and what dims are truley critical, your time frame etc.

[halestone]

If you use a cnc mill

as i look at your part in drawing i would cut my flat stock in 6" lenghts X the hieght of your pic part then place in a vice and up agenst a stop so that the hieght is now horizonal and clamp just bellow center to allow you to cut step. Next i would program machine to use a 1/8 carbide two flute cutter to generate two .2 holes, one step and radius. when get done with that op relocate part upside down from previous op and on a pin in one of the holes, reclamp and run secound step and radius now all the parts are complete to size next mount parts one at or two ant a time invice jaw against a pin and drill 2 remaining holes dburr job done

[Hellbringer]

do they have to be aircraft percision..... no there is some play. it is track links for a model dozer and the 2 holes on top are where the track pads whould bolt to. so there is some play.

thanks again guys for the ideas
mike

[Geof]

The amount of precision is irrelevant. On a CNC machine you can get +/-0.0005" precision just as easy as +/0.05" in the same machining time.

The important thing for reducing machining time is fixturing. Perhaps I did not explain my approach clearly enough.

When you do multiple parts like I suggest you reduce the time wasted on tool changes. With single parts there is a tool change for every tool for every part; if you have five parts lined up in the machine there is one tool change for every five parts per tool.

Similarly if you do single parts there is a loading operation for every part; with five parts there is one loading operation for every five parts.

If you grip the stock as I suggest for the first operation so it is possible to machine the top and all the way around the perimeter it is not necessary to square anything up beforehand; five sides are machined in this operation and all are perfectly true because nothing has been re-fixtured in between.

In addition you have saved a lot of time because you only need to cut the original material into lengths for five parts; this reduces the number of cuts and time spent preparing the stock.

It does not matter what way you look at it the fastest way to bang out parts is with the correct multiple part fixturing if the part design makes it possible.

[KOS]

Originally Posted by Geof The amount of precision is irrelevant. On a CNC machine you can get +/-0.0005" precision just as easy as +/0.05" in the same machining time.

Well if he does more of the work manually then the precision is very relevant. If he can throw them on a bench sander to make the radius and do it in multiples at a time and they dont have to be within a small tolerance than there are other faster ways to machine it. Same goes with a drill press.

I do agree that the fixtures are very important though, as you have mentioned.

None are really right or wrong, just which way to make them based on what tools are available and how accurate they need to be in the end. If not all the work is done on a cnc machine then it is important. If he decides to do them all on his mill then it would no longer be a question.