Surface grinding angle brackets to fit into channel?

We need angle brackets to attach extruded 45° mitered channels together (similar to a picture frame).

We will either make custom angle brackets (shearing, punching, and braking) or buy a used surface grinder and modify off-the-shelf angle brackets. Modifying the off-the-shelf brackets involves surface grinding 3/32" off both sides so the 5/8" wide bracket will fit into the 7/16" channel. The thickness of the bracket is 3/32", so there isn't much metal to be magnetized. I attached a drawing of the angle bracket. My question is, can it be done, and/or is it more trouble than it is worth?

If we had it, I'm sure we would use the surface grinder for other projects in the future.

Any insight is much appreciated!

How many are you doing at a time? One or two you would need to block in with some steel drops, but If you stack multiples they'll support each other, and make sure the fence on the side of the chuck is up as high as you can get it without intersecting the wheel. You don't want to rely solely on the magnetization to hold them. That just keeps them down. Nesting them with each other or steel blocks keeps them in place.

Surface grinding seems like the worst way to thin those parts. That's a milling job, or better yet just contract the bracket to a sheet metal company. You'll be dollars (a lot of them) and time (ditto) ahead to let a pro do that part.

Thank you for the response. We buy the brackets in quantities of 100. So, 100 at a time. Yes, they do nest nicely together. I'm sure there are a lot of variables, but how much would you take off each pass?

HoneyGrids said:

Thank you for the response. We buy the brackets in quantities of 100. So, 100 at a time. Yes, they do nest nicely together. I'm sure there are a lot of variables, but how much would you take off each pass?

Click to expand...

Really depends on what wheel you have, if you are running coolant, etc. though I agree with Milland that if you are doing so many, it would be cheaper to have them made to the correct size.

Yes, from past experiences modifying stock (on a mill in a vice) wasn't the way to go, but I have no experience with surface grinders, so I was hoping it might be different. That said, why is it the worst way to thin the angle brackets?

Surface grinders are for precision work where you have to remove something between zero and maybe .01". Sure, they can remove a lot more, given time and necessity, and they commonly do, but you're talking almost a tenth of an inch. Milling territory for sure.

Conrad Hoffman said:

Surface grinders are for precision work where you have to remove something between zero and maybe .01". Sure, they can remove a lot more, given time and necessity, and they commonly do, but you're talking almost a tenth of an inch. Milling territory for sure.

Click to expand...

Gotcha. Thanks!

HoneyGrids said:

Thank you for the response. We buy the brackets in quantities of 100. So, 100 at a time. Yes, they do nest nicely together. I'm sure there are a lot of variables, but how much would you take off each pass?

Click to expand...

Qty (100) at a time ?
Make print, post down below to have someone laser cut and bend them.

Milland said:

Surface grinding seems like the worst way to thin those parts. That's a milling job, or better yet just contract the bracket to a sheet metal company. You'll be dollars (a lot of them) and time (ditto) ahead to let a pro do that part.

Click to expand...

Have you considered Out-sourcing the bracket to a "Short Run Stamper" to make this Sheet-metal Bracket. Check in the "Thomas Register" for suppliers. The Surface Grinder is not a milling machine and if you persist your headed for a process that you will find is too expensive and not the proper way to proceed. The Surface Grinder is for precision work. This is a Sheet-metal Bracket. Removing .0002 to .0005 down feed at a pass is normal on a Surface Grinder.
You could order strips slit to width from a sheet metal supplier, shear to length; build a drill jig for the holes and form on the Brake.

Roger

Milland said:

Surface grinding seems like the worst way to thin those parts. That's a milling job, or better yet just contract the bracket to a sheet metal company. You'll be dollars (a lot of them) and time (ditto) ahead to let a pro do that part.

Click to expand...

Have you considered Out-sourcing the bracket to a "Short Run Stamper" to make this Sheet-metal Bracket. Check in the "Thomas Register" for suppliers. The Surface Grinder is not a milling machine and if you persist your headed for a process that you will find is too expensive and not the proper way to proceed. The Surface Grinder is for precision work. This is a Sheet-metal Bracket. Removing .0002 to .0005 down feed at a pass is normal on a Surface Grinder.
Or; Order strips slit to width from a sheet metal supplier, build a simple drill jig, shear to length and form on the brake.
Roger

Agree fast, efficient would be to mill and grind only what you need precision. If part needs +- .002 and difficult to hold then to finish .010 .005 on the grinder might be due.

Mill only if you can make specs.

Surface Grinding you would buch them to make a full wheel width of parts, and long-way down one leg, then turn the part and long run the other leg. pulling perhaps .002 at each travel both ways down feed. having two dressers, one at near - .045 and the other at finish target. You would long and down travel only ..no crossing on the part.

If you have to run two operations mill & grind then grind only might prove better. XX not.

Ops! my bad grinding 3/32 off each side would be a lot to make mill speed. likely you would never match the mill with a surface grinder.

If you have regular orders of batch 100, have someone make them exactly as you want them.

If you have on hand a batch of 100 that need re-sized, they can be done on a surface grinder and *possibly* as fast as milling.
Might be ahead, depending how heavy the burr is from milling.

there are a lot of variables, but how much would you take off each pass?

Click to expand...

If you make a substantial end-stop block, and stack the corners in a cheveron down the chuck with another block made to jam agains the stack, against a tall rail on one side and another block on the opposite....
Then, i would take 3 roughing passes per edge of .030", and one clean up/finish pass with whatever is left (.004?)
I'd position the parts so the "arrow head"/corner point is toward the up-lifting side of the wheel. Wheel pushing down legs first as it climb cuts)
If that ran well, i might even go down to 2 roughing passes of .040" and finish pass whatever is left (.014"-ish)
Flood coolant required.
Set the infeed at about .003 - .005" per table reversal, and let it run. (You can calculate time from that - figure both sides and time to clean and re-stack 4x 2 to rough each side, 2 to finish)
36 grit fairly open wheel, probabbly I hardness.


If you don't get it (wheel spec, table speed, coolant) figured out to develop a step in the wheel instead of a ramp, you will be dressing a lot off the wheels when the ramp gets too wide.

For security, hopefully you will be using a fine pole electric chuck. But a good FP permanent mag would work

The thing is, even if those parts are $1 each (seems high?) You will have way more than $100 in grinding them.
Also, do both legs have holes?
Due to the way parts heat and squirm on a surface grinder, location holes can wander a bit, even though the brackets end up precisely on target. Holes might no longer be exactly centered, or even co-axial (co-planar) with each other.

Or you could make a fixture with locating pins/hold downs to clamp & keep them centered, one at a time, point up, and straddle mill between two spaced cutters, climb cutting on a horizontal mill.

Realistically it's all more expense than the parts likely cost.

smt

SendCutSend can make these for you quick-turn to try it out. They'll laser the blanks and bend them.

Metal Bending and Forming Guidelines - SendCutSend

Then if you like the result get it quoted from other shops for a better price.

Grinding you may want a 3hp or larger spindle motor so to pull perhaps a 1 1/2" (or wider) wheel.
Running one leg with down feed and long travel you would be best served with the widest stack of parts.
With a 1 1/2 wide wheel you might run 15-16 parts
a 2" wheel 20-21.

Up side:
Rough grind one leg, skim dress and skim grind that leg.
turn part stack and R grind other leg, skim dress and skim part stack.

Qualify the ground side for flipping, perhaps wire brush to remove bugs and burrs.

flip the stack bottom-up and run the other side.

Making two simple diamond holders just the right height will be an asset because the part finish size will be a gage spec number to each dresser, so way less travel to the dresser and no need to measure the part.

The skim dress and skim finish will take almost no time and will greatly reduce the need /time to qualify the second side.

You should/might lay down a .430 x 2" x 10" parallel at your bump rail so as not to stress the bump rail screws.
Knock in a bump block to the close side, perhaps 2" x .430 x 6"

You might put a parallel clamp on the end of the stack (at the right end) so the magnet will hold that end down as a group.

Thank you, everybody, for chiming in. The surface grinder is out. Outsourcing is the way to go.

I'm amazed at how inexpensive it is to have parts laser cut. SendCutSend is 0.78 cents each (I think I was overpaying locally). That includes the holes we were going to punch! We have a 25-ton press in-house, so bending them isn't a problem.

Check local grinding shops who have a Blanchard Rotary Surface Grinder. It would take longer to set them on a chuck then grind them. Grind one side and flip on the chuck. To make it affordable, buy 500 or 1000. You could set them side by side touching each other. You could have them put a ring around them for safety, Then afterwards put them inside a tumbler to deburr the sharp edges, or have an employee use a belt sander.

HoneyGrids said:

Thank you, everybody, for chiming in. The surface grinder is out. Outsourcing is the way to go.

I'm amazed at how inexpensive it is to have parts laser cut. SendCutSend is 0.78 cents each (I think I was overpaying locally). That includes the holes we were going to punch! We have a 25-ton press in-house, so bending them isn't a problem.

Click to expand...

A win for common sense. Rare these days...

[Also, you joined ten years ago and these were your first posts? Now that's getting the feel for a board before getting involved]

HoneyGrids,
How large an order did you place?
Asking because I may have a part needing similar work.
Buck.

michiganbuck said:

HoneyGrids,
How large an order did you place?
Asking because I may have a part needing similar work.
Buck.

Click to expand...

It depends if you use their parts builder or send a custom file. Although the custom file I uploaded is similar (slight change in hole placement) to the part I created with their parts builder, it is double the price.

I encourage you to try out their parts builder since it is effortless to use, and the quotes are instantaneous.

Here are the price difference screenshots. For 100, it is $1.52 compared to 0.78 cents. I found a workaround to use their parts builder and get the holes where I want them.




Also, they sent me a 10% coupon after I registered. "SENDCUTSAVE10"