[Wooden Payload]

Hey everyone,

Just wanted to see if I could get some pointers on making finishing passes on the outside profiles of the parts I work on. I write toolpaths for and operate a PCNC 1100 for the company I work for, and up until now, I don't know of a good way to fixture a part for a full depth finishing pass on the outside edge. The obvious limitation is that the vice jaws are in the way when trying to do this.

The best way I have found to do it thus far is to make a simple fixture which I bolt the parts down to after some features are already cut into the part. But, for runs of about 2 or 3 parts, making a fixture isn't all that time efficient. For parts I don't use fixtures on, I am usually left with using tabs on the part which I cut off and file down, leaving unsightly marks every so often.

As an example, a part I'm working on right now is a 2.5" x 4" 6061 0.125" thick aluminum plate. I'd like to cut all of the inside features, and then do a finishing pass on the outside, but apart from making a fixture, I don't know of a way to do it. Many of the parts I work on are panels or thin parts with holes/cutouts in them, or engravings. Really not a whole lot of 3d geometry.

Any advice? Or am I stuck with making simple fixtures?

Thanks!

[Wog]

Fixtures can be very basic. Just some scrap aluminum with a series of tapped holes. If most of your parts are say 1/2" or 1" centerline to centerline holes, make a fixture plate with a grid of 1/2"-apart tapped holes and use it for many different parts. It is sacrificial, so just mill your finish pass .01" lower than the part.

[Peter Neill]

Can you bolt into it from underneath?
In the Toolroom we have a few sets of these fixture plates that are held in a 6" vice and used on an old Bridgeport Interact for machining EDM electrodes (mainly), but will hold anything you can bolt from underneath.

[Wooden Payload]

Fixtures can be very basic. Just some scrap aluminum with a series of tapped holes. If most of your parts are say 1/2" or 1" centerline to centerline holes, make a fixture plate with a grid of 1/2"-apart tapped holes and use it for many different parts. It is sacrificial, so just mill your finish pass .01" lower than the part.

Definitely a good idea. I actually worked on a pretty nice fixture plate a while ago, but never finished it. Also, the hole patterns are typically not even, which is mainly why I still haven't used it. I think the tapped holes in a scrap piece will be the best bet on this particular part, thanks. I guess the issue that I see coming up is a part with a random hole pattern, and no good geometry to reference off of. In this instance, I would have to spend the time to make a fixture with a square surface to indicate off of. I just had a part yesterday like this and I had to let it go with a crappy surface finish on the outside. Luckily it was a prototype and didn't matter a whole lot.

Can you bolt into it from underneath?
In the Toolroom we have a few sets of these fixture plates that are held in a 6" vice and used on an old Bridgeport Interact for machining EDM electrodes (mainly), but will hold anything you can bolt from underneath.

I like that idea. This particular part doesn't have any tapped holes, but having through holes in a standard fixture plate for bolting from the bottom could be really useful in some situations. Thanks for the idea!

I realize complaining about making simple fixtures is a little ridiculous, but with the variety of parts I do in such small quantities, and with the rate at which revisions are made, it hasn't been very practical to make a fixture for every part. Thank you for your replies, keep 'em coming! :cheers:

[Wog]

One way is to drill for tapping the same hole pattern (just 2 holes unless it's a large piece) in .375" or .5" thick aluminum plate. Use the same width and length as your .125 plate, that way your X&Y zeros stay the same. For just a few parts, I'd tap the holes with a cordless drill with the plate still mounting on the mill.
Hope that makes sense.

[SquibLoad]

A method that has worked very well for me has been using vacuum clamping and simple 1/8 or 1/4 inch locating dowels.

Most everything I machine needs full outside profile cuts, and no other method has worked as well.

Here's how: Make a simple flat plate, of wood, acrylic, aluminum, etc., then drill a hole in the side or bottom of the plate for a 1/8npt quick-release fitting, and two dowel holes, either 1/8 or 1/4in depending on the size of the part. Drill matching holes in the bottom of your stock to be machined. They only need to be 1/16 in or so deep. Insert the dowels in the plate, apply foam tape to the plate in the outline of the part, hook up a vacuum source, and away you go! Works great, and can be controlled by a simple foot switch or ball valve for very quick part changeout and repeatable positioning. If it is a small part and plate, I clamp this plate in the vise, if it is bigger than can conveniently fit in the vise, then I bolt it to the table.

You can use the dowels as reference points for indicating your fixture position for repeatable placement, and even set up G54.x work offsets for each fixture.

I plumbed my vacuum source in permanantly to my table, and now have vacuum clamping available all the time.

[Steve Seebold]

A good way to do it is to leave an extra 1/4 inch on the bottom of the part, do all the finishing operations then flip the part over and fly cut the bottom off.

[howecnc]

What Steve said but I have gone as thin as .125 to cut off the bottom later and make soft jaws frequently for odd shaped parts for the removal of the extra and secondary features.

[WOTDesigns]

This video shows "vise fixtures" which are fast, free, and easy. For your part you probably don't even need to machine the locating features. if you have a square pocket just drill and tap a couple 2-56 holes into some scrap so they fit inside the pocket (2 along one axis and 1 on the other), still and tap 2 more holes to hold the part down. I do it all the time and it takes about 5 minutes to drill and tap all 5 holes. The part will repeat within a thou or two.

https://www.youtube.com/watch?v=FQKY...e_gdata_player

Another thing I do when there are no holes for screws other than a slot is drill three holes that match my locating threads into a piece of scrap slightly larger than the slot. Put screws through the holes then through the slot and push the part against them as I snug them up. This way locates and holds with only 3 screws. fast easy and free.

[Wooden Payload]

Thanks for all of the replies everyone, definitely learning and lot, you all have really cool ideas.

A method that has worked very well for me has been using vacuum clamping and simple 1/8 or 1/4 inch locating dowels.

Most everything I machine needs full outside profile cuts, and no other method has worked as well.

Here's how: Make a simple flat plate, of wood, acrylic, aluminum, etc., then drill a hole in the side or bottom of the plate for a 1/8npt quick-release fitting, and two dowel holes, either 1/8 or 1/4in depending on the size of the part. Drill matching holes in the bottom of your stock to be machined. They only need to be 1/16 in or so deep. Insert the dowels in the plate, apply foam tape to the plate in the outline of the part, hook up a vacuum source, and away you go! Works great, and can be controlled by a simple foot switch or ball valve for very quick part changeout and repeatable positioning. If it is a small part and plate, I clamp this plate in the vise, if it is bigger than can conveniently fit in the vise, then I bolt it to the table.

You can use the dowels as reference points for indicating your fixture position for repeatable placement, and even set up G54.x work offsets for each fixture.

I plumbed my vacuum source in permanantly to my table, and now have vacuum clamping available all the time.

I really like this idea because of the infinite variability you have in the shape of the part. I guess a limitation might be internal cutouts in the part? For instance, a plate with a hole pattern in the interior of the part, as well as an outside profile. I think I might look into making one of these, though. I suppose the internal geometry could be blocked off somehow. Thanks for the idea!

A good way to do it is to leave an extra 1/4 inch on the bottom of the part, do all the finishing operations then flip the part over and fly cut the bottom off.

What Steve said but I have gone as thin as .125 to cut off the bottom later and make soft jaws frequently for odd shaped parts for the removal of the extra and secondary features.

For rectangular/square parts this would work awesome, I just can't see making soft jaws for every random little part I make. The company I work for pretty much strictly does internal prototyping, and any time there is an order for a large quantity, we send the parts to an actual machine shop. The parts I work on are short notice, quick turnaround, one off parts that in many instances will be revised and remade within a couple days of making the first part. Makes me a little angry some times...

[keebler303]

For the thin stuff, you might get away with a vacuum chuck or even just some good quality double stick tape. Just slow down a bit on your profile cut so you don't rip it loose. I have also used wood as a spoil board which is handy to just shoot a woodscrew into wherever it is convenient.

For thicker stuff, normally the stock would be around 1/8" too thick and you would grab that 1/8" in the vice. Do your profile cut, flip the part and clamp on the finished profile, then face mill the remaining material to bring the thickness to spec.

Matt

[Steve Seebold]

What Steve said but I have gone as thin as .125 to cut off the bottom later and make soft jaws frequently for odd shaped parts for the removal of the extra and secondary features.

1/8 inch could be good. It just depends on how how tall your part is.

[thefu]

not to toot my own horn but i use .060 for most parts with lower ipm's, anything with heavy cuts i use .125 carrier material

[Wooden Payload]

1/8 inch could be good. It just depends on how how tall your part is.

I agree, in certain situations it could be good. I know I would be wary of trying to go to 1/8" to face off, just because my closest parallels are exactly 0.125" below the top face of the jaws, and the step jaws that I have also have a 0.125" step. I'm sure there is a way to shim it up so you don't cut into the jaws though.

I started working on a simple vacuum setup yesterday with numerous locating pins. Obviously, this isn't an end all solution, but it's certainly something to add to the bag of tricks. If any of your are also interested in this, I can post some pictures of the solidworks model I made for now, and possibly a half way machined version later today.

Thanks again for all of the good ideas. Collaborating on stuff like this makes me realize how little I know and how many cool ideas other people have. :cheers:

[Steve Seebold]

You could also make some soft jaws to hold your part if you think you're getting too close to the vise jaws. Most of the time if I need to have something to hold onto on the bottom of the part, I will leave 1/4 to 3/8 of an inch. If you're working on a part and only holdong 1/8 inch and you hit the vise jaws with your end mill, you not only screw up the jaws, you also screw up the bottom of your end mill.

I would rather have a little more to machine off, and finish 5 sides of the part before I cut the bottom off.

[rowbare]

You might also want to look at Mitee-Grip from Mitee-Bite Products Co.. From the product page:

Mitee-Grip is a heat-activated wax-based compound embedded in precision paper, coated on nylon mesh or in a stick form. This holding media maintains parallelism on precision parts. Mitee-Grip is very useful when machining thin or hard-to-hold parts and allows machining on five sides of a workpiece without using a clamp.

bob

[Steve Seebold]

You might also want to look at Mitee-Grip from Mitee-Bite Products Co.. From the product page:


bob

I have never used Mitee-Grip. It looks like some neat stuff. My question though is, how do you get it off?

[rowbare]

I have never used Mitee-Grip. It looks like some neat stuff. My question though is, how do you get it off?

It is wax-based so a bit of heat will take care of it. I imagine someone using it regularly would keep a little hot plate or electric frying pan around.

bob

[MichaelHenry]

It is wax-based so a bit of heat will take care of it. I imagine someone using it regularly would keep a little hot plate or electric frying pan around.

bob

I just bought some and the instructions say to clean up with soap and water or alcohol.

McMaster-Carr sells it if anyone is looking for a good source:

McMaster-Carr

It's the "heat-activated" clamping compound on the bottom of the page. McMaster doesn't advertise vendor names, but the stuff I ordered from them is made by Mitee-Bite.

I haven't had a chance to use it yet.

Mike

[twocik]

The art of fixtures..... It'd be fun to start a thread on just fixtures. :cheers:

As for a fixture to help you out, this is definitely custom to the part you're making. I make fixtures for just about every part I make because I'm doing them in mid to large quantities. Making a fixture takes time, some times a lot of time, and can really save you on time. If you're running a bunch of the same parts, you can get the talon grip vise jaws that only need .06" as the carrier. You'll need to switch the jaws out for a finish operation, but if your run is big this will save a ton of facing time and tool life.


Here's a fixture I made for tiny parts and works great.








This one might be hard to see. This is a press fit fixture that is cut exactly to the length of my part and then pinched in between the jaws. This is a spot, drill, tap and slit mop.