Machinist

[Lawrence London <lfljvenaura@gmail.com>]

How do you accurately locate a vee groove with a mill?
http://www.practicalmachinist.com/vb/general/how-do-you-accurately-locate-vee-groove-mill-339446/

It's pretty easy to measure V grooves with a known diameter pin and the right micrometers or indicators.

I think you're asking how to locate a work piece in order to cut a V-groove.

If so, scribe the desired centerline on the work piece, make a cut, clamp a precision pin in the cut and measure to datums.
Adjust as required.
Take another cut, measure, adjust.
Repeat as required.

put in a construction hole, ream a dowel, pick up on that at the angle.

Cut the groove, and mill the sides until it's in the center.

touch off on a "good" vee block that is positioned on the table along with the work.
plus or minus what ever indicator you choose.... Can;t do much better ...

If the diameter of the endmill is known accurately, you can calculate where the 'top corner' of the endmill is relative to the bottom corner (.707106 * diameter). So if you touch off the bottom corner of the rotating tool on the top of the stock, using a thin piece of shim stock to feel the moment the tool starts to grab, then you can calculate how far to move the tool to bring the top corner level with the top plane of the part, then add the additional distance to lower the tool to the centerline of the stock.

You cannot effectively make any use of the quill for the cutting, total vertical adjustments would be done with the knee elevator. I suppose you can 'reverse engineer' where the quill should end up having made the initial setup as described, and so then you could back off the quill and make progressive cuts towards a known destination.

<>

The op said "accurate" but didn't say "how accurate". A method to use a flat endmill, if something is not required to be super-accurate, but within say 0.005", layout with Dykem, mark CL of v-groove with calipers etc, tilt head (for example rotating head ccw to left), check with angle-block, retract and lock quill, align corner of cutter on scribe (using magnifying glass), turn on machine and move knee up till it just starts to cut, adjust x to scribed line while barely cutting (using magnifier); to make groove, move knee up (lock axis not in use) an appropriate cutting depth (material removal increases as the groove is made deeper). If the endmill is not large enough for the depth of the groove, index it down/over equal amounts with the knee and x to remove the "waste" at the top right side of groove.

Errors are going to add up and compound using an endmill at 45', dunno how accurate and repeatable one could reasonable expect.

Tilting the head 45 deg on a BP by yourself is a pain; I clamp an approx 18" piece of 2x4 in the vise (table/vise moved all the way to the left for ccw head tilt) at an angle such that it rests against the casting on the joint between the motor housing and casting (near the switch) after about 15 deg is reached, and use it to lower and raise the head; I put a socket on the worm gear and basically use the knee to raise and lower the head, just using the wrench and worm to "keep up" with raising it by the knee. You have to periodically smack the 2x4 with a hammer to keep the 2x4 at the correct angle to be in contact with the head. This also allows you to fiddle with the locking screws during the process since they seem to need need tweaking during tilting, unless you loosen them a lot (not recommended).

<>

check this out might help
TIPS #393 How to Cut a V Groove on the Bridgeport Mill tubalcain - YouTube

<>

If the head is tilted you can take a shallow cut, measure with respect to a feature such as a part edge, and then dial in the correction. In order to do this you must do your vertical feed with the knee only, not the quill.

A tilted part is a bit trickier. Best bet is to use trigonometry to figure the horizontal and vertical max feeds to reach your desired location and V groove depth. Then "touch off" from the two part edges to get your zero points. The upper tilted edge will be your zero for depth and the lower tilted edge will be your zero for horizontal feed (in the same direction as the zero was set).

It's best to stop before final depth to measure and re-check your calculations. If you have a lot invested in the piece it's also a good idea to practice on scrap first.

>\<>

Another thing I forgot to mention is that if you have a small straight clearance cut at the bottom of the Vee (and all good V-blocks should have one) you can set a stop for the bottom (end) of the piece and turn the piece 180° before making the final cuts. The groove will be centered automatically in the piece. This only works if the diameter of the cutter is wider than the faces of the Vee.

<>

Simple geometry, if you tilt the part 45^o then you just have to divide/multiply all the vertical and horizontal offsets by sqrt(2). Mr Pete does give a pretty good explanation without blowing up your head. The idea is to locate the center with the corner of the end mill and move depth/sqrt(2) in horizontal and vertical. for a 90+^o "V" things get a bit more complicated and you need to make a separate setup for each side cut. You cannot cut a 90-^o "V" the same way, because of the undercut.

<>

For the sine bar you don't need vees. Most sine bars are cut with rectangular cuts and the screws that hold the rounds in place are at a 45 degree angle to hold them against the "bottom" and side of those cuts.

OK, for the Vee blocks. Most Vee blocks are symmetrical so you will want the vee cuts in the center. I would first make two Vee block blanks with the same width and height. Then make a 45 degree fixture with a solid stop on one side, AKA a Vee block. This fixture Vee block need not be accurate except for the 45 degree angle. Clamp it on the mill table and align it with the X axis. Now...

1. Put one Vee block blank in the fixture Vee block and touch off the corner of the end mill on a scribbed center line.
2. Move the table on the X axis to place the quill off the side of the Vee block blank so you can lower the quill.
3. Move the table on the Y axis toward the Vee block blank by the depth of the desired vee.
4. Lower the quill by 1.4 times the desired depth of the Vee. This places the end of the mill a little short of where the second side will be. You can go a bit less than this if you want.
5. Lock everything down and take the cut.
6. Remove the Vee block blank and reverse it.
7. With the quill and Y axis at the same settings, cut the second side.
8. With the quill and Y axis at the same settings, make two cuts on the second Vee block blank.

Those two blanks should have vees cut in them with the same width and depth. And both of them should be centered in the blocks.

It may be a good idea to make rough cuts a few thousandths short of the final sides on both blanks first and then do the final, finishing cuts with the Y axis and the quill moved by those extra thousandths.

This method will leave a bit of extra metal at the apex of the vee so it also may be a good idea to either drill a lengthwise hole at that point (before milling the vee) or to use a slitting saw at 45 degrees to remove it.

You could use an angle vise instead of the fixture Vee block I called for. It would need to be set parallel to the X axis and accurately set to 45 degrees. Your blanks would be set against the fixed jaw AND against the bed of the vise or against a parallel shim resting on the bed. The idea is to tilt the work, not the head/quill.

<>

How about calculate the width of the final vee, scribe those lines on the block, set the cutter at the correct angle, and mill out until you cut to the two lines.

<>

scribe lines are good to about +/- 003