Fixture Feature (or, how I learned to stop worrying and love tooling plates)

Over the past 4-5 months I've been making a wide variety of different parts for a 6-axis robotic arm I'm working on. With at least 20 unique milled parts in a variety of shapes and sizes, this project has forced me to learn how to make my workflow from 3D model to first part off the machine a lot more efficient, as most of the parts I make are quantities of one or two. So I thought I would share some of the things I've learned along the way I wished I knew about sooner.

A couple weeks ago I spent some time making a small tooling plate to help make some parts used for the wrist joint of the robot. I wish I had made one of these sooner as it is looking like it will be useful for all different kinds of parts. It was made from a roughly 6"x6"x3/4" piece of 6061. I decided to make it as a vise fixture because it would only be needed for relatively light machining, and this would allow me to use either the vise or tooling plate without having to pull the vise or re-zero things. I started by cutting two pockets on the back side of the plate, so that I could drop it into the vise and have it locate to the same spot every time without any other tools.

Attachment 243814

The plate was then flipped and placed into the vise as it would be used and the top machining was done. The top was milled flat to a depth of .200", leaving a lip on the top and left sides so that stock can be brought square to that corner. If you preferred, any other corner could be used as well. The top and left corners were milled to be exactly 5.5" and .2" from the bottom left corner. I then drilled and tapped a grid pattern of 10-32 holes over the plate (the T/C tapping head earned its keep on this one!). The rows of holes are spaced .5" apart in X, and staggered in groups of two alternating rows in Y. One row was .5" apart starting .5" from the top lip, and the other was .5" apart starting at .75". The spacing was chosen to work with the Mitee-Bite fixture clamps I've accumulated a collection of from previous projects. The clamps work with an offset of .250" from the stock edge, so with the hole pattern I can place clamps on any piece of stock that is a multiple of .5" in X, and a multiple of .5" or .25" in Y.

With this fixture plate I was able to quickly set up and machine some pieces which required machining virtually all of the interior space of the part, as well as profiling all the way around. Here is a (mostly) finished part.

Attachment 243816

The way this worked was to do it in two setups. One with slightly oversize stock gripped around the edge would perform all of the interior machining, including a pocket and placing holes. Because the fixture plate uses a .5" grid, it is easy to add holes to a part or use existing holes to locate it. These would be used to both locate and hold the part in the second setup, which machined a profile all the way around the part. I set this up in my CAM program by making two copies of the part, located at the two positions on the fixture plate, so that I could have both setups on the fixture at the same time. This reduced tool changes per part and would also allow me to make copies quickly (though I only needed two in this case) as each machine run would produce one finished part. Here is a preview of what the toolpaths looked like:

Attachment 243818

And here is what it looked like after running them:

Attachment 243820

These are not particularly complex parts by any means and there are many other ways one could approach this, each with their own advantages and disadvantages. I appreciate seeing walk-throughs of how other people have solved problems as it helps to build my mental library of ways to approach a new part. This approach saved me the trouble of having to locate the part origin multiple times (once you have located the fixture, everything else comes from that), and I could do all different kinds of profiles without having to use soft jaws.

fixtures are awesome , i love wrapping my head around that type of thing
Those types of cam clamps are one of my favorite , I generally make them to suite the job . Even on round parts they work great if they have a radius cut into them to match the part . They are perfect for whipping together a fixture with a few pieces of stock and maybe a few pins .
Another favorite of mine is making wedge clamps with the use of countersink bolts . I'll make wedge clamps between two parts or what not . Other times I'll turn some round stock groove it , drill , countersink then part off and split it , then hold it together with an o ring in the cut groove . Works great for clamping internally on bores . I do a lot of production type stuff so simple clamping with the least amount of wrenching is necessary .
A lot of complex parts can be machined with only one clamp if its well thought out

Very cool,
I have used these for a while now and found this method fast and easy to setup and use in both design and cam ops.
As you mentioned you can add holes to design to hold parts or use existing opening with screws and washers or other holders.
"mini pallets " I call them was the reason for buying tc unit and learn tapping setups. 110 holes on each and I make 3 or 4 at a time.
I make them in both aluminum and acrylic in a couple different sizes but mostly use a 5x6 that fits in vise best.
The holes 0.5 on center and squared edges. I use a machinist square clamped to pallet for aligning parts and tighten screws down.
Also have these as fixtures in cam software along with screws and washers to include in models for tool path avoidance and checking
Just need to be carful on depth to avoid milling pallet surface to much or needing to resurface it.

Some pictures of my pallets

Attachment 243852

Attachment 243854

Anyway great to see others using this method, I was wondering what others did.
md

I'm running a job now that makes 21 pieces in a single set up. If I ever run it again, I'll make a second fixture so I can have one in the machine making parts and the other out on the bench being unloaded and reloaded.

I'm making a washer for some parts I make for my remote control race boats and I can't buy one that's thick enough so I figured if I have to make them anyway, I'll just make them different.

I made them out of 3/16 aluminum and since I am making them myself, I decided I didn't want just a plain 5/8 round washer so I made them 5/8 hex with a .090 chamfer on them. It may be extravagant, but it will look good.

Someone told me a long time ago, "if you can't make it right, make it pretty".

Are you facing the sides or just cutting them from the 3/16 stock and leaving the mill finish?

Quote:

---

Originally Posted by kstrauss

Are you facing the sides or just cutting them from the 3/16 stock and leaving the mill finish?

---

I'm just using 3/16 X 3/4 bar stock. I suppose I could have used 1/4 inch stock and machined them top and bottom as well, but this is model boats, not rocket science.

Quote:

---

Originally Posted by mountaindew

Very cool,
I have used these for a while now and found this method fast and easy to setup and use in both design and cam ops.
As you mentioned you can add holes to design to hold parts or use existing opening with screws and washers or other holders.
"mini pallets " I call them was the reason for buying tc unit and learn tapping setups. 110 holes on each and I make 3 or 4 at a time.
I make them in both aluminum and acrylic in a couple different sizes but mostly use a 5x6 that fits in vise best.
The holes 0.5 on center and squared edges. I use a machinist square clamped to pallet for aligning parts and tighten screws down.
Also have these as fixtures in cam software along with screws and washers to include in models for tool path avoidance and checking
Just need to be carful on depth to avoid milling pallet surface to much or needing to resurface it.

Some pictures of my pallets

Attachment 243852

Attachment 243854

Anyway great to see others using this method, I was wondering what others did.
md

---

MTD - Can you email me the solid model of the Tormach vise, or is there a D/L for it somewhere?

Quote:

---

Originally Posted by BAMCNC.COM

MTD - Can you email me the solid model of the Tormach vise, or is there a D/L for it somewhere?

---

Tormach web site has a decent selection of their fixtures models pre-drawn and filed under documents and drawings. "solid models"
Car lane and other fixture suppliers also have some of theirs available.

btw the bolts, nuts , studs shown holding vise ARE NOT included in my cam models :)
Wow do some of those take up so much memory and slows things to a crawl at times... so be careful
The ones I add like screws and washers, plates... I keep them very simple so not to use memory for no reason!
Hope this helps
md

Oh, nice didn't know that. I'll check them out.

I won't normally model with it, but wanted to check it out anyways. It's going to be hard for me to use HSMWorks for the Mill I think, but will try it. I can whip out a 2.5D part so fast in Rhino it's scary, not sure I'd ever make up time on simple things with HSMWorks.

My PC has 32bg of ram, so a few bolts won't bog it down ;)

Quote:

---

Originally Posted by BAMCNC.COM

Oh, nice didn't know that. I'll check them out.

I won't normally model with it, but wanted to check it out anyways. It's going to be hard for me to use HSMWorks for the Mill I think, but will try it. I can whip out a 2.5D part so fast in Rhino it's scary, not sure I'd ever make up time on simple things with HSMWorks.

My PC has 32bg of ram, so a few bolts won't bog it down ;)

---

You can't use HSMXpress/HSMWorks with Rhino anyway. They work ONLY with Solidworks and Autodesk Inventor.

Regards,
Ray L.

lol. yes I know. I'm sponsored by HSMWorks and own Solidworks - Just saying though... Atleast until I fully learn the capabilities of HSMWorks.

Quote:

---

Originally Posted by BAMCNC.COM

lol. yes I know. I'm sponsored by HSMWorks and own Solidworks - Just saying though... Atleast until I fully learn the capabilities of HSMWorks.

---

That's cool nice software., Is this new?
Your videos in the past showed you struggled a bit with this process.
md

Like anything, it's always harder to RE-learn a new way to do something. I started out with Rhino and RhinoCAM, and you pretty much can't get farther away from Solidworks and HSMWorks than Rhino CAD & CAM.

I just tried to watch a demo from HSMWORKS where they advertise to draw and cut a part in only 4 minutes. It looks great, but there was no sound.

I'm just starting a series for HSMWorks, been to busy to get down there and start playing with it. The series will more or less involve going from an idea, to a part in your hand. Also will have Rhino VS Solidworks, and RhinoCAM vs HSMWorks - Then many people can make up their mind as to what you ACTUALLY need for cad/cam software.

I love modeling with Rhino! Rendering work is way fun once you get the layering and lighting effects down. I've worked with solidworks in the past and yup it is a cad program that does a lot, but it never gave me that feeling of freedom. My brain has thoroughly enjoyed the flow of Rhino solid/surface--->IGES---->Sprut! Through all the struggles of getting to the point where 3D 3 and 4 axis milling work and fixture design are not a problem anymore with this combo I believe that I actually have expanded my own consciousness You know in an "Exit The Matrix" kind of way, but not quite like eating LSD blotters, drinking mushroom tea and listening to the Doors kind of way LOL!

Sprut is mind altering!
I treat these programs like my kids would a game. If you fail you try a different direction and note where the traps are.
Try not to fight to much. I know I did not long ago setting up multiple tools for thread milling .
I just about had the program unstable. then I step back erased what I had and went at it different.

These are all complex programs not phone apps
Its a challenge to learn them and keep the running even. I spend many hours late at night playing these games
md

I still haven't tried thread milling. That is one thing I need to try.

Quote:

---

Originally Posted by BAMCNC.COM

I still haven't tried thread milling. That is one thing I need to try.

---

Thread milling isn't any more difficult than any other type of milling other than you're moving in a spiral instead of a straight line.

I did a thread job a couple of years ago and it was a learning experience for me. I was cutting an internal right hand thread and I made the mistake of cutting the thread from the bottom up in a clockwise direction. It cut a beautiful thread and if the mating part had a left hand thread on it, all would have been perfect. It turned out that when cutting from the bottom up on an internal thread, I needed to move in a counter clockwise direction. Once I figured that out, the rest of the job went along perfectly.

When I cut a thread, I don't take several passes. I do it all in one pass.

I'm getting ready to do some 10-32 threads on some brass parts. I like to cut brass because I can run it dry and there's no coolant mess.

haha yeah, Just watched a video on Shadon HKW's channel, he turned a long lead screw... backwards! lol It's how we all learn.