S
swarf_rat
Titanium
- Joined
- Feb 24, 2004
- Location
- Napa, CA
- Nov 8, 2015
- #1
VMG 35 deg diamond bit in a straight holder. Normal procedure on my Prototrak is to set the X and Z by taking cuts and measuring the diameter and face (all tools are offset to reference tool). This works fine for X but I can't think of a way to measure Z. You can't face with the diamond bit in a straight holder. I could try guestimating the point position with a magnifier and then offset the radius and maybe get close.
Some way I haven't thought of to do this?
Finegrain
Diamond
- Joined
- Sep 6, 2007
- Location
- Seattle, Washington
- Nov 8, 2015
- #2
I've wondered the same thing, and look forward to seeing what others do for this case. I've done a test cut in a setup piece and measured as best I could but would be nice to have a more definitive process.
Regards.
Mike
alphonso
Titanium
- Joined
- Feb 15, 2006
- Location
- Republic of Texas
- Nov 8, 2015
- #3
I've always treated these as a threading tool. Just eye ball the center(point) and go on.
J
jhearons
Cast Iron
- Joined
- Sep 16, 2003
- Location
- riverside, ca, usa
- Nov 8, 2015
- #4
Touch the shank of the tool to the face of the work and set Z. Shift Z by 1/2 the width of the shank. If for some reason the tool has a jogged head, refer to the manufacturers catalog (or measure ahead of time ) to find the amount to shift.
S
swarf_rat
Titanium
- Joined
- Feb 24, 2004
- Location
- Napa, CA
- Nov 8, 2015
- #5
On my threading tool holder (laydown inserts) I offset to the edge of the insert because in most threading jobs it doesn't really matter where the thread starts, only that the tool doesn't hit a shoulder. But I am trying to contour with the diamond insert, comp offsets by the radius but expects to know where the (virtual) left edge is. Without that the contour will be offset relative to features cut by other tools. An optical comparator held over the tool is about the only way I can think of.
I guess one could program say a 45 degree taper with a left hand reference tool, then chase it with the V tool and adjust Z offset to match. One peculiarity of the Prototrak control is, cutter comp is only applied during a running program so it would be a little tedious.
S
swarf_rat
Titanium
- Joined
- Feb 24, 2004
- Location
- Napa, CA
- Nov 8, 2015
- #6
jhearons said:
Touch the shank of the tool to the face of the work and set Z. Shift Z by 1/2 the width of the shank. If for some reason the tool has a jogged head, refer to the manufacturers catalog (or measure ahead of time ) to find the amount to shift.
Good idea, I'll try that and see how close I get. There would be a build up of tolerance: measure width, measure edge, divide, subtract the tool radius. But at the least a quick way to get a starting point.
C
Clive603
Diamond
- Joined
- Aug 2, 2008
- Location
- Sussex, England
- Nov 8, 2015
- #7
Maybe a block with a sharp V cut-out matching the tool angles made with its centre line a known diatance from the side would be more accurate and worth the extra trouble. Think I'd arrange things so the block could be strapped to the tool shank with the V wrapped snugly around the tip then bring the whole kit and caboodle up close to the end of the workpiece or other suitable calibration point and measure the gap. Measuring is likely more repeatable than simple touch off. I guess a loose part carrying the V fixing to a shank with appropriate clamping arrangements would be easiest to handle. Single screw through clearance hole large enough for sufficient fine adjustment ought to work. Sounds a ton of trouble to do but if it just works may be worth it over cut'n try.
Only times I've ever done anything like this touching the shank worked fine. But good enough was within 20 thou or so.
Clive
S
swarf_rat
Titanium
- Joined
- Feb 24, 2004
- Location
- Napa, CA
- Nov 8, 2015
- #8
OK, I set it up as suggested by jhearons, then checked it by cutting a 45 deg angle using a left hand tool with the same tip radius (same tip radius should remove radius comp from the equation). Then I chased it with the VNG bit. I had to adjust the Z offset by about 0.001 to get it to dust the angle, so it was pretty close.
S
SeymourDumore
Diamond
- Joined
- Aug 2, 2005
- Location
- CT
- Nov 8, 2015
- #9
Actually, since this tool is no good for anything other than finishing a profile that needs it, I'd say that picking it up very accurately in Z is essential.
There are 2 ways that I can think of.
First the easy one: If you have an optical comparator, just create the face with your known tool, and then use the VNMG to plunge a shallow groove
into the OD somewhere. Record the Z position. Take the part to the shadowgraph, measure the distance from the face to the groove center, add the value to the offset
register. Simple
Without a shadowgraph:
Create a known groove with a grooving tool, say .100 wide and center being @ .100 from the face.
Then take the VNMG, position it somewhere inside the groove, and then move backwards until the tool touches the back edge.
Zero your operator Z position, then move forward until you touch the front.
Read position screen, move back 1/2 the amount and bang, now you're .100 behind the face.
I'm never more than .002 off with either of these methods, and I do set up quite regularly with this tool.
You must log in or register to reply here.