Gallery, Projects and General > How do I??
How do I - locate centre and position end mill? - basic milling.
CrewCab:
When I decided to have a go at single point threading I bought a few bits of Delrin (or Acetal), it's an engineering plastic, pretty cheap and easy to machine ........... so good to practice with.
CC
zeusrekning:
All right let me put my poot in. How would I make this part in my home shop? That can be answered so many different ways. Multiply that by the number of different ways other people would make it. Then again figure in all the different ways dependent on what tooling is available. See where this is going. What im getting at is this is how I would make this part in MY shop.
First my assumptions.
1. The center bore diameter is critical.
2. The location between the center bore and the bolt circle and slots are critical.
3. That the outside profile is not so critical.
4. Material is to correct thickness.
5. Material is not correct width and saw cut to length.
6. The part is symmetrical with the bore being centered (two slots , one on each end).
7. Looks like large bore my have a counter bore on the opposite side.
8. I assume the part is 1/2" thick, 5" wide 8" long.
9. All dimensions have been taken and a sketch made.
So how I would go about it.
I think 1/2" thick by 5" wide is too tall to stand up and machine the edges.
1st op. I would arrange my vise jaws so that I can hold on the 5" long sides (by putting the jaw on the front of the mobile jaw).
I would hang the part out of the side of the vise about 3/8" and machine the 8" long side using a common 1/2" dia HSS endmill.
I would then take the part out of the vise and deburr.
Then put the machined edge against the fixed jaw and machine the two 5" sides bringing the 8" length dimension in.
Again remove and deburr.
Now you should have a plate with 2 parallel ends and one long edge square to the two ends.
I would then hold the part long ways again and machine the 4th edge to dimension.
Now you have a plate to the correct outside dimensions all square. :headbang:
Obviously this would be easier if you had material to size but again, MY SHOP. I never have aluminum to the correct size.
Next, With my jaws in the usual position in the vise I would use parallels to space the part up so that I can grip on at least 3/8" and leave a bit of material sticking above jaws.
If there is enough material to make a fly cut I would if not I wouldn't.
I would then find the center of the plate using an edge finder and zero the good ol' DRO.
Then spot drill slightly all major features (all hole centers and the center of the slot start and end points.
I would then drill all holes to size, drill 4 holes for the slots. Depending on the size of the slots I would either use a drill the same diameter as the width of the slot or the next available size down if it is an oddball dimension for the slot width. Lets call these my slot holes.
Next I would use a 3/8" endmill and cut from the center of one slot hole two the other. Id prob do these in two cuts of 1/4" each. Making sure to lock the table down in X. Repeat for the other slot. Then with a good sharp 3/8" HSS endmill I would move to the center of one slot hole. Move over .04" or so and make a cut to the center of the other slot hole at full depth. (Making sure to conventional mill not climb cut) If you are not familiar figure out the difference between these two terms.
At the end of that cut I would move over the center of that slot hole +.04" and cut the other side. Then measure. After that ...... Measure again.
Your slot should be .045" narrow if all cut good. Do the math and repeat using number needed. Side point. Many DRO's have the feature when you can store datum points. It would be nice to store all feature points that you center drilled earlier. This is nice b/c then when doing the 1st slot you just move to zero of slot hole one, it will read (X0-Y0) and move over equidistant amounts.
Then do the same for the second slot.
I would then drill as big of a hole as I could for the center bore. For me this would be a hole saw prob in the 2-3/4" to 3" diameter range. I would then put the boring head in. I would make a skim cut and measure, cut and measure and so on till the bore is where it needs to be. If there is a larger counter bore I would probably machine it the same way as the bore was done. But I would use a boring bar with the leading edge as square as possible. If you use a regular bar with plenty of leading edge relief you will end up with many small steps in the bottom of the counter bore. This is the reason for wanting a square edge. I would also set my quill stop assuming that the counter bore depth is not super critical.
I would then flip the part over (after deburring) and find center of the large bore. I would then move to all four holes of the bolt circle and counter bore using the closest size endmill I have available, again using the quill stop for depth.
For the angles on the outside If not needed I would omit them, If needed I would first lay them out with my combination square and scribe.
Before we proceed , this may not be considered the best way but It works for me. And I'm assuming it would fit and work but may not once at the machine.
I have a set of tall jaws, I would put these in the vise. Then I would hold the part so that the corner I plan to remove is sticking above the vise. Using a parallel laying flat on top of the vise jaw I would get the scribed line parallel to the top of the vise jaw and tighten the vise. Then using an endmill I would machine down to the line. Then repeat for the other three corners.
And for the fine print.
Im sure I left something out, if not it is a good day. And If all went as planned and I didnt leave anything out Id go buy a loto ticket. :lol:
Tim
Ok I went back and reread your question. Not sure if You wanted all that I posted above or not. But for the slots it is almost always better to use a smaller endmill than what the width of the slot is finished to. The enmill will want to pull left and right and will cut poorly and prob oversized. Same for keyways,
kvom:
Tim's advice is all good. (I think he may have switched the edge milling on the sides, as not many home shop vises will open 8", but that's a nit).
In looking at the motor and bracket, I would opine that your tolerances are pretty wide. You need to get the 4 bolt holes close, but since the bolts have washers you will have no issues if they are a bit larger than the bolts. The center hole needs to clear the motor face and leave the ventilation slots open, and the bracket slots need to match where they will be mounted. Once again you almost certainly have a pretty wide tolerance. The bracket thickness likely just needs to be enough so that the nose of the motor doesn't protrude.
What I am saying is that for anything you make you can decide how accurate and precise it needs to be. Spending hours making that slot accurate to .001" will be time wasted it .1" suffices. What people are saying here is that you should know HOW to get the .001 precision when you need it.
Having a boring head for your mill is a useful thing when you need a hole larger than your drills, esp. if it needs to be a precise size. For this bracket, it would be much faster to set it up and cut than doing it on the lathe with the 4-jaw. You can also enlarge a hole with the part on a rotary table using an endmill, but once again the setup is more time consuming.
Navigation
[0] Message Index
[*] Previous page
Go to full version