Fixturing and toolpaths for noobs

[JimDawson]

You have 3 counterbored holes in the part, use them. Use a scrap piece (fixture plate) in the vice. Face it off and drill and tap the hole pattern into the piece. Clamp the workpiece to the fixture plate, drill and C-bore the holes. Screw the work to the fixture plate and remove the clamps. Do all the machining from one side.

Rather than facing off the back with a fly cutter, use a 3/8 endmill and take it all in one pass using a facing routine. Around 2800 RPM, 18 IPM, 60% stepover.

 

[koenbro]

You have 3 counterbored holes in the part, use them. Use a scrap piece (fixture plate) in the vice. Face it off and drill and tap the hole pattern into the piece. Clamp the workpiece to the fixture plate, drill and C-bore the holes. Screw the work to the fixture plate and remove the clamps. Do all the machining from one side.

Rather than facing off the back with a fly cutter, use a 3/8 endmill and take it all in one pass using a facing routine. Around 2800 RPM, 18 IPM, 60% stepover.

Yeah I like this (and @Boswell ‘s) plan best. I have a LMS fixture plate and can use an MDF piece sandwiched between the Alu stock and the fixture piece. Or remove the fixture plate and attach the MDF directly to the bed.

I use this all the time on the CNC router btw, but was reluctant to use MDF as I think the lateral forces are quite high.

I think this must come up very often -- what kind of material do y'allz use as a backer?

 

[JimDawson]

I think this must come up very often -- what kind of material do y'allz use as a backer?

It depends. Sometimes MDF, sometimes aluminum.

Here is an example of a MDF backer and the parts bolted directly to the table. The large cap screws use the T-slots, the smaller ones are drilled & tapped into the MDF. Work material in this case is 1/2'' steel, this started out as one solid piece about the size of the MDF.


Here is an example of using an aluminum fixture plate with the work screwed down to it. This also has a tooling plate under the the aluminum backer.


These are the parts that were machined on the above setup


Here is a chunk of 4140 bolted to an aluminum backer in the vice. Punch press connecting rod.


I have many more examples, but I think you get the idea. You are only limited by your imagination. Just think through the whole process before you make any chips.

 

[JimDawson]

Here is another one for you to think about. I'll be making this in the next day or so.

6'' OD x 1'' thick, 6061 aluminum, holes are 5/16 through. Face, drill, pocket, bore, and profile.

How would you do it? I'll post pictures of the setup when I get to it.

 

[Parlo]

I would tackle this as most have said before if you only want to use a mill.
1. Face both sides to thickness.
2. Drill holes.
3. Drill tapped holes in sacrificial plate + one reference hole in the centre for future use.
4. Screw the blank to the plate and press go.

Check the drawing for the tolerance on the thickness, you may be able to use stock thickness material and skim the faces - only if machining is required on the print. This will give you the edge when quoting as you will save 2 operations and maybe 10% on material cost. It may be worth a quick call to the client to establish the importance of the 1" dimension.

Quick tip. Always drill the parts befiore making the fixture. This way the fixture can be left in position ready for production.

If I had access to a lathe then I would consider starting with tube and facing/chamfering to thickness and roughing out the counterbore within a couple of mm. Then drilling the holes on the mill. And finishing on a fixture as above.

The method chosen all depends on variables such as material cost / time / machine availability / quantity etc...
Larger quantities will lend themselves to multiple fixturing.

 

[koenbro]

Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?

 

[Parlo]

Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?

You could rub all the parts on a scothbrite pad when finished machined. I use a scotchbrite disc on a random orbital sander for a satin finish. Either way, any slight scratches will be disguised. So I would machine the thickness first.

 

[JimDawson]

Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?

In general, as machined is acceptable. Most times mill finish and some minor scratching and surface blemishes are acceptable. We are not trying to make mirrors. We normally only face from one side for thickness. The exception to this would be when there is a callout on the print for a surface finish. Since 99.9% of our work is for our own in-house use, we set the specs on the surface finish. Most parts are as machined and normal debur. Some are vibratory finished. All of our aluminum parts are anodized or powder coated, the stainless parts are as machined.

In the case of the part above, only the face shown needs to be skim cut, just to make it perpendicular to the bore. The OD and the back do not matter.

 

[Boswell]

This sounds like a fun game, I'll play!

1. clamp stock to table on sacrificial spacer (MDF) with clamps that do not interfere with the interior feature. ensure that MDF has roughly corresponding hole in center for step 3 clamping
2. Mill the interior feature
3. Relocate clamps to inside of part ensuring that they do not interfere with exterior feature. Move clamps one at a time so part does not shift and clamps to not obscure drilled hole locations
4. Mill exterior feature and drill/tap holes

 

[JimDawson]

I would tackle this as most have said before if you only want to use a mill.
1. Face both sides to thickness.
2. Drill holes.
3. Drill tapped holes in sacrificial plate + one reference hole in the centre for future use.
4. Screw the blank to the plate and press go.

Very close to the way I'm doing it.

Check the drawing for the tolerance on the thickness, you may be able to use stock thickness material and skim the faces - only if machining is required on the print. This will give you the edge when quoting as you will save 2 operations and maybe 10% on material cost. It may be worth a quick call to the client to establish the importance of the 1" dimension.

In this case this is for in-house use so the 1'' is a ''suggestion'' It will actually be a bit thinner, like about 0.995 or so.

Quick tip. Always drill the parts befiore making the fixture. This way the fixture can be left in position ready for production.

We drill parts on the fixture all the time, just be very careful of the drill depth so not to screw up the threads in the fixture.

If I had access to a lathe then I would consider starting with tube and facing/chamfering to thickness and roughing out the counterbore within a couple of mm. Then drilling the holes on the mill. And finishing on a fixture as above.

The work could be done on the lathe, but I'm too lazy to stand there and do it.

The method chosen all depends on variables such as material cost / time / machine availability / quantity etc...
Larger quantities will lend themselves to multiple fixturing.

Absolutely. Given this is a 1 off, for an in-house project, I have a lot of flexibility.

This sounds like a fun game, I'll play!

1. clamp stock to table on sacrificial spacer (MDF) with clamps that do not interfere with the interior feature. ensure that MDF has roughly corresponding hole in center for step 3 clamping
2. Mill the interior feature
3. Relocate clamps to inside of part ensuring that they do not interfere with exterior feature. Move clamps one at a time so part does not shift and clamps to not obscure drilled hole locations
4. Mill exterior feature and drill/tap holes

This is the time to use an aluminum spacer. I gave your method, using MDF, some thought, and in this case the process can be simplified by bolting down to a scrap aluminum piece.

So here is how I'm doing it. This is not the only or best way, just how I decided to do it given what I had to work with.

First a quick video of the simulated operation

First the fixture plate. I found this on the aluminum shelf, was a fixture plate for another project. Roughly 6x6x0.5


Mount it up in the vice and roughly locate the center hole. The hole is about 0.377, so a 3/8 dowel pin in the drill chuck makes a good center finder.


Face and drill & tap the 5/6-18 mounting holes. I can only use 4 of the 6 holes because the existing top & bottom countersunk holes are roughly in line with the part holes. If four 5/16 cap screws won't hold the part then I'm doing something wrong.


Next locate a fixed point that won't change during machining. This way if you have a power fail or otherwise lose zero, then you can easily recover. I used the top, right corner of the vice, and wrote down the DRO position. Z 0 is the top of the part, so is easy to reset.


X/Y coordinates of the top corner of the vice relative to 0/0. A vice movable jaw makes a good scratch pad for a Sharpy.


Center up by eyeball, precision is not required at this point, +/- 1/16 or so is close enough. Plenty of excess material to remove. Clamp to the fixture plate and drill the six 5/16 holes 1.050 deep. This puts the drill point through the material, but doesn't damage the previously threaded holes in the fixture plate.


Now take a skim cut on the face, about 0.005'', using a pocketing routine. Now we have a flat surface to work from and that face is complete. That divot in the lower right (not the one circled in black, the one below it) of the picture is what we commonly call a ^%(&&#*


Now bolt the part down and remove the clamps, in that order. Now is ready for the rest of the operations.