Custom V-blocks?

Hey,
I'm pretty new here and I have a grinding question so I figure I'd ask here. We have a DoAll G1 surface grinder in our shop and I have some parts that I'm trying to figure out how to finish. I don't have much experience grinding so bear with me. Picture the parts as a tube of chap stick but only about 1/3 of the length. These parts need to be ground on each end to meet OAL, flatness, and perpendicularity callouts. The datum surface is the OD. I have an idea in my head that I think would work but I don't know where to find something like this. In my head if I had a block with multiple V's that was almost as thick as the part is long. I could put several parts in it and tighten them down with a flat edge, grind one side, flip the parts, and then grind the second side to the overall length. I think this would also give me the flatness and perpendicularity callouts I need to hit. I was thinking I could even use two of these v block things, one on each side and some wedge clamps in the middle to double the amount of parts I could do at once. I drew a picture of the basic setup because I'm sure I'm doing a poor job describing it. Anyway, does something like this already exist and is readily available? If so, any tips on finding it? If not, do you guys know of anyone who makes custom v-blocks and could do this? We have something similar in our shop that we made in the past but we aren't a tooling shop and I'm looking more accuracy than I feel we can make. I'd also be happy to hear any other ideas you may have on how to grind these parts. Any input is greatly appreciated. Thank you!!

Having a mill you might drill a line of hole (or a double line ) into a long block and add a set screw holes from the outer shell to hold a row (or two rows) of parts. That would be easier than grinding the Vs and making another bar to hold down. The mill could be very well tramed… or you could after drilling in one set-up just set screw in a well squared part and with indicating it skim grind the sides after mill-drilling to square up. Yes you could ream the holes but IMHO that wiuld b overkill. I would lay a strip of printer paper under the block to protect my chuck.

To make the one you show one could dress the V into the bottom of a surface grinder wheel and grind a row of Vs In line with the cross feed..V bottom notch not needed because the rounds would never touch there. Yes redress and go back to skim the Vs so they would all be the same. The Vs would not have to be very deep or even perfect centered , just all near all the same so the hold down would hold them..

Some grinder hands might set a normal V block on the chuck, diamond dress the wheel face and then hand bump the first side of such parts to the wheel face. secone side could be bumped also but that would not control length,

michiganbuck said:

Having a mill you might drill a line of hole (or a double line ) into a long block and add a set screw holes from the outer shell to hold a row (or two rows) of parts. That would be easier than grinding the Vs and making another bar to hold down. The mill could be very well tramed… or you could after drilling in one set-up just set screw in a well squared part and with indicating it skim grind the sides after mill-drilling to square up. Yes you could ream the holes but IMHO that wiuld b overkill. I would lay a strip of printer paper under the block to protect my chuck.

To make the one you show one could dress the V into the bottom of a surface grinder wheel and grind a row of Vs In line with the cross feed..V bottom notch not needed because the rounds would never touch there. Yes redress and go back to skim the Vs so they would all be the same. The Vs would not have to be very deep or even perfect centered , just all near all the same so the hold down would hold them..

Some grinder hands might set a normal V block on the chuck, diamond dress the wheel face and then hand bump the first side of such parts to the wheel face. secone side could be bumped also but that would not control length,

Click to expand...

Thanks for the input. I'd like to have these made somewhere if I can. Do you know of a shop that specializes in making this kind of thing? If not, I can take your suggestions and see if we can come up with something in our shop. I'm just worried about the precision involved. The drawing calls for .0002" perpendicularity and .0002" flatness to the O.D. for each side of the part.

nate8649 said:

Thanks for the input. I'd like to have these made somewhere if I can. Do you know of a shop that specializes in making this kind of thing? If not, I can take your suggestions and see if we can come up with something in our shop. I'm just worried about the precision involved. The drawing calls for .0002" perpendicularity and .0002" flatness to the O.D. for each side of the part.

Click to expand...

Looks like a job for a wire EDM. They make their own tooling all the time.

Square up your block and send it out for HT. Then grind it flat and send it out for EDM to cut the V's.

.0002 is tight.. You might carbide drill, drill and ream or just HSS drill a one hole test block to see if .0002 might be made with holes. mild steel Ok for test block.

EDM suggested sounds good. You might drill holes and then let the EDM shop finish to Vs. EDM all in one set up and Vs would be close.. Then tickle grind to square up if needed. Yes drilling holes just to save that time at the EDM shop

Yes you could make in one piece with EDM cut Vs having screw holes so not needing the top clamp bar..Might make it with top and bottom side rails (like an H) so you could flip to grind two sides of parts. Grinding wheel would be between the set rails of the H.

* Very likely parts will slide with the separate top clamp bar. Yes I have used such top clamp holders.

Might need a double screw and going through a solid bar so grinding would not move them in the fixture if close length is needed for grinding part ends and with not solid to other ens support they would slide. Going through to set on the chuck they would not slide, Going through and set on a sheet of copy paper would protect the chuck..but the copy paper would not be good for another use.

Or just WEDM circles to hold the part that are .0002 over in a hardened block that's height is 0.125" less than the part is long. You could have a block with as many circles as you can afford the wire guy to put in.

Holding like that with those tolerances is going to depend on the cylindricity of the part. I would have that fixture ground square then have the vees ground after machining. This way you know everything is straight. Also, I would have pins put in for the parts to rest on, that way your u can clean one side then flip and adjust to where your final will be.

I have made bump together blocks that held to very close end squareness. Yes for one-ups or two ups only as bumping in to a row of parts would not hold them all tight.

Yes just a pair of blocks with a precision V ground into it. I have made these for stand up grinding ends. I put a shim across and between setting on the chuck to set bottom end off the chuck. Just one bump block bumping to a solid block works well also.

For very small diameters perhaps 1/32 to .005 or so it is good to travel only one way..from the grind side... or they chatter and can break if hard.

Grinding full wheel not Incrumential cross feed is best.. With moving (cross) a diameter width after a few parts to get fresh wheel bottom..Back to back of wheel re-dress.

* With the ops design it might be good to have a diamond at about the part height and dress a skim before the last .002 (or so) finish pass. The diamond perhaps set off chuck could be set as a gauge height so dress + .001 (or what) down-feed would make part finish height good.

for much surface grinding an off chuck adjustable height diamond can aid faster and more accurate grinding. Often better than an overhead diamond.

I occasionally do things similar for work, modifying parts to be short .005" as machine set-up rejects. (For automated machinery that inspect parts)

This is what I came up with, although I haven't made it yet. There would be a V block clamp on the end, and you flip the entire unit over to grind the bottom side of the part parallel to the top.

The top Vee isn't needed, just the one on the end. I was just thinking of ideas in CAD for a more useful tool.



Sent from my XT1053 using Tapatalk

Are all of the OD's the same, and held to the same .0002 tolerance? If so, that makes it much easier. However, I would caution screwing a screw into a .0002 OD unless you plan to use brass screws. You could EDM V's in one block and V's in another block, and haven them bolt together in a few places.

You could also make the fixture and hang it off magnetic parallels, dust one side, and flip over and dust the other.

Another way to do this, if you have the capability is an OD grinder and a collet setup. I'm not sure on the specifics of the parts you are running, however I'm thinking this would be the best bet

H shape lay down fixture:

Say the part is 3/8 diameter and 1/2 long ?
For that one might take a piece of bar stock 5/8 x 1 x 6" long. Drill a row of 1/4" holes where the finished 3/8 holes or V are intended to go. On one 5/8 side drill two screw holes for each 3/8 part. send it out to wire EDM the 3/8
holes or Vs..

lay it on a mag chuck and grind a little over 1/2" x 1/8 depth long way down the 5/8 side face on both sides. Screw hold a part and grind one end to test for squareness.. Shim and grind one 1" side to make dead square the holes on first side.. flip over and skim the other side. likely a fixture for 12 parts.

*Yes before this is made, a one part block cold be drilled on the mill and tried with set screws holding to test the concept of simply using a hole rather than a wire EDM hole or V..Yes truing the block for squareness would be done on the surface grinder

For a long run the H fixture might be hard or case hard.. for a short run likely mild steel
Yes if the part is a material that would be damaged by a steel screw a brass point or brass screw would be used.

Yes the fixture would be like a lay down Parallel with a row of holes.
Yes the depth of the 1/2 by 1/8 depth could be perhaps 1/2 by 1/4 deep on one side.

Again} the fixture in post #1 is not a good design, a lot of work and wont work.

.0002 squareness on a part where the length and diameter are nearly equal? How are you going to check it? Any vee block fixture you design, I'd do a design test with a one piece fixture before committing time and resources to a larger fixture.

I'd do it in a very high quality rotating fixture, such as a Harig or Newbould. That assures squareness to the centerline of rotation but not flatness. This leaves your problems being loading the part into the vee block or collet and squareness of rotation to axis of travel.

Regardless of how you do it I see cleanliness as your biggest problem.

What material and hardness?

With not having time to grind chuck then do flat grinding far away from the bump rail.. The top of the chuck closest to the operator is often the truest area.
Grinding a 6" long fixture tale your time and use coolant so not to burn and warp.. Yes a hand spray bottle is fine.

We did this exact thing for grinding carbide rods. We made a matched set so we can swap them in and out of grinder.

Steel blank, grind bottom, drill & tap holes, wire EDM vees. We made 5 clamps (not shown) with vees to hold the rods.

They work very well.

Thanks for all the input. I made a model of my idea. I didn't include pins to rest the parts on but I would plan on adding them. I contacted a Wire EDM tooling shop and they said they can make these. The things in the middle of the design are wedge clamps so they tighten on both sides. It holds 20 parts.

plastikdreams said:

Holding like that with those tolerances is going to depend on the cylindricity of the part. I would have that fixture ground square then have the vees ground after machining. This way you know everything is straight. Also, I would have pins put in for the parts to rest on, that way your u can clean one side then flip and adjust to where your final will be.

Click to expand...

I plan to add pins to my design, thanks.

Spyderedge said:

I occasionally do things similar for work, modifying parts to be short .005" as machine set-up rejects. (For automated machinery that inspect parts)

This is what I came up with, although I haven't made it yet. There would be a V block clamp on the end, and you flip the entire unit over to grind the bottom side of the part parallel to the top.

The top Vee isn't needed, just the one on the end. I was just thinking of ideas in CAD for a more useful tool.

Sent from my XT1053 using Tapatalk

Click to expand...

I like the idea of being able to flip it without taking the part out of the clamp

bigbee67 said:

We did this exact thing for grinding carbide rods. We made a matched set so we can swap them in and out of grinder.

Steel blank, grind bottom, drill & tap holes, wire EDM vees. We made 5 clamps (not shown) with vees to hold the rods.

They work very well.
View attachment 195536

Click to expand...

Very cool, similar to what I want to do.

A wire EDM,

As long as its a good set-up the machine could finish both sides with a good fixture.

JS said:

A wire EDM,

As long as its a good set-up the machine could finish both sides with a good fixture.

Click to expand...

Surely expensive method though?

I like fixture the OP has come up with, a lot of parts can be ground in a setup like that.

To check the parts I would make a fixture comprising a vee block tipped about 10 degrees off vertical with a ball bearing held at the bottom in the center of the part. an indicator at the outer edge of the opposite end of the part would measure perpendicularity.

QT: gbent [.0002 squareness on a part where the length and diameter are nearly equal? How are you going to check it? Any vee block fixture you design, I'd do a design test with a one piece fixture before committing time and resources to a larger fixture.]

QT: sable [As long as its a good set-up the machine could finish both sides with a good fixture.]

I would take a cold roll steel block perhaps 2”long x 1”wide x.060” taller than the part. Set it up on the mill to dill and ream two or three (part) holes a little larger than the part (or a very close fit). drill and tap two holding screw holes for holding each part. (Yes making one 6” long would take little more time perhaps two hours to make…)

Grind the H shape so the recess is .035 deep on each side. Check the squareness of the holes and tickle grind the top and bottom of the H fixture to make dead square (if needed). Lock in parts and run a few sets to test the H holder concept.

This is a fixture for finishing two sides.
if you cant make dead square .0002 then make the same with EDM Vs.Yes if you could not make .0002 with the drill and ream test the very same H fixture could be sent to the EDM shop to make Vs. in the same holes.

I would mark each side of the H fixture with "minus .003" (or what perhaps -.003 and - .007) to show the needed below the height oh the H fixture to make part size.. that way after wheel dress so you can hand touch the fixture and know what dial number makes length size.

Yes CRS may not last for ever so needing a log run harder material(heat treat)might be the better choice.

For a very long run double holding screw holes would be put in both sides. The EDM VS would not be Vs but diamond shape so when the wall opposite the holding screws became washed out from wear the other side would be used.