Order of operation - General considerations

I have a feeling this is a question that will be answered with "Experience will provide the answer." Anyway, when looking at a drawing, are there any general guideline as to what should done first, next, etc..? It seems like a silly question, but my limited experience has revealed a number of "I should have done this before I tried to do that". Like should I bore the hole before I finish the outside diameter? Should I center drill all the holes, then drill them all, then ream them? Should I finish surfaces before drilling/milling? Just looking for general ideas.

Peace.

Big before little, saw off the end of the bar, machine it. Lastly, admire it.

Tough to give an all inclusive answer but mainly just take your time and think through the part before you start. The on-the-fly machining does work, but can often be done better with a little planning.

In general minimize the number of setups you need to do. I try to avoid starting the part until you have all the tools you need to finish it, because from experience, I will need to take that part off the machine while I'm waiting to get the right tools, and then there is a setup induced error. Try to machine the more critical, more likely to be messed up features near the beginning of the part (when reasonable) so that if you do scrap the part, the number of hours lost is minimized. Think about how you will hold the part as you move along. If you only have square mill jaws, maybe cutting a weird shape part on top and flipping it over is not the best way to do it.

For example, I didn't plan out a part very similar to this one very well...



So what could have been a 1 or 2 operation part turned into me chucking into the lathe 5 or 6 times. I was able to indicate in with a tenths indicator, so the error was very small, but it took many hours to do so that were completely unnecessary with a little forethought.

Macardoso -
Thanks for the insight.
Could you list the steps you should have take with that part? I know it would open a host comments from others, but the ensuing conversations would be of great benefit to us novices.

Order of operations is influenced by a number of factors and there is no hard and fast set of rules. The operations and consequences of those operations needs to be thought through for each project. The order is also influenced by the work holding options that are available. The number of setups and required registration accuracy between the setups also influence the order of operations.

For instance, it is possible to perform a number of operations and find that there is no practical way to hold a part for the final operations. When boring a thin walled part, I find it easier and more accurate to bore the internal diameter first and deal with flexure in the wall with the o.d. turning. Another example would be making a washer from a sheet of metal. I would face the material to the required thickness, drill the hole, and rough cut a blank from the plate. Then mount the blank on a mandrel and turn the o.d.

I recall a past thread where the poster was making a three piece assembly which had a bullet shaped exterior and the threaded pieces were threaded together. There was a good discussion about order of operations in that thread.
https://www.hobby-machinist.com/threads/new-project-im-in-over-my-head.70311/#post-588974

That's something that comes with experience, with lathe work you try to do as much as possible without taking the part out of the chuck
Mark

Starr256, sure!

So here is the model of the part I had issues with:



It was a servo motor mount which held two back to back angular contact bearings. The concentricity of these bores was extremely important (.0002 to .0004 deviation max) as was the diameter. The depth of the space between the bores was not as critical.

Here is what I did:

1. Square stock to size (I used my 4-jaw on the lathe since my lathe has more HP)
2. Rough out the central bores on the lathe and ream the center hole to size all the way through (this was my locating feature for other operations)
3. On the mill, drill the 4 corner holes and start the two center bolt holes (used a long reach endmill to counterbore them)
4. Flip the part and drill the 2 center bolt holes from the other side (didn't have a drill long enough to go through from one side, again make sure you have the right tools before starting a part.
5. On the lathe, finish bore the large hole in the center, as well as the two smaller diameters behind that, and the motor pilot diameter
6. Flip the part and finish bore the second bearing seat

All counted (not including the flips to square the rough stock) I had to indicate the part on the lathe to a very tight tolerance 3-4 times as well as indicate on the mill twice. All of these flips induced some error in the bore alignment. I was fortunate to hit the concentricity within .0003 but this was not a good way to do it. If I needed to make more, this would have been my order of operations:

1. Square stock to size
2. Drill and counterbore all holes from 1 side (buy a longer drill) on the mill
3. Rough and finish all diameters from the one side
4. Flip the part on the lathe and bore the final bearing seat.

This only requires 2 precision alignments for the setup and would take way less time. If it were acceptable to press in an tubular insert to achieve the smallest diameter, all boring could be done in a single setup would would be ideal.


EDIT: That flat on the top was the last operation and it was done on the mill. It wasn't a tight tolerance feature.

starr256 said:

I have a feeling this is a question that will be answered with "Experience will provide the answer." Anyway, when looking at a drawing, are there any general guideline as to what should done first, next, etc..? It seems like a silly question, but my limited experience has revealed a number of "I should have done this before I tried to do that". Like should I bore the hole before I finish the outside diameter? Should I center drill all the holes, then drill them all, then ream them? Should I finish surfaces before drilling/milling? Just looking for general ideas.

Peace.

Click to expand...

The question is not silly, and in fact is one of the more important aspects of machining. Experience does help, and there are some good answers posted above. Sometimes I spend as much time thinking about how to machine a part and order of operation as I do actually machining the part. This is especially critical when using CNC equipment.

To answer specifically with regard to holes on a manual machine, I like to spot drill, drill, tap/ream without moving the table. So doing each hole as a completed operation before moving on to the next hole, this minimizes location errors. This assumes that you have a flat surface to work with to prevent the drill bit walking off to the side. Where possible I normally do all of the work on holes as the first operations, then do other machining operations as needed. Holes make great things to put bolts through to anchor the part for subsequent operations

Normally it's best to ''machine'' the entire part in your head before ever making a chip. For simple stuff you can kind of do it on the fly, but for more complex parts it may require sitting down with the raw material and the print and going through it step by step. You have to be able to hang on to the part and reach the target area with the tool bit. Sometimes you find that you need a little extra material to hang onto to be able perform an operation and then remove it in a later operation.

As said above, do as many operations as possible in a single setup to minimize location errors.

JimDawson said:

Normally it's best to ''machine'' the entire part in your head before ever making a chip

Click to expand...

This.