Making a fitted case for a tool

[enl_public]

I spent a little time (ok, took a 1/2 hour process and dragged it out over several days grabbing photos and screen shots, but…) making a case to document the process for those that may be interested.

The process is similar with most tool chains, but this was done with Inventor/HSM. Everything can be done with the free version (student/education/hobby), and is nearly the same with Fusion360. The work flow is a little different with SolidWorks, but the net result is the same.

First is the prep. Meet the Starrett 425 M&E 3" caliper.

I am the second owner , my father having been the first, and it dates to just post-war. It came to me when he was lightening the load before moving about 25 years ago.

I make up a dimensioned working sketch before touching the CAD system, as it is quite a workflow breaker measuring while working on the model. The sketch allows me to build an accurate model of the tool, or as accurate as needed to make the case, given that I cut a few corners here. The only special features here are the arcs, and to make a neat job of the case, they should be matched. So, out came the radius gauges:

5/16" was a bit small (see the single point of contact near the lock screw, and the gap at the left of the gauge), and 11/32" had two point contact with almost no gap at the midpoint of the arc. (The actual radius is 0.335+/-0.005", measured with a three point sagitta gauge) For a neat fit in the case, the larger radius is desired.

The sketch:

(more to follow)

[enl_public]

Next came the CAD model. I modeled the tool as a single solid, rather than by modelling the individual parts. In this case, it was a little easier, but it is often easier or necessary for other reasons to model the parts and assemble them in the CAD system.

First, a boundary/outline. This is for the tool with the jaws open a little, and comes in useful later when using the model to make hollows in the bottom and top.

Then, the profile of the tool outline (with the jaws open a little) is drawn and extruded to a solid

After that, other features go on: the lock knob on the front, the grip on the back, and the lock wedge/screw end on the back. This is one place I cut serious corners. These are modeled simply and with maximum dimensions, rather than to accurate form, making the lock know a cylinder and the thumb grip a rectangular block.

These featured are modeled by selecting the appropriate face of the part as the work plane and dimensioning from the existing features.

Once that was done, I stretched the features. This is another shortcut. It is better for a general purpose design to sweep the part when making the cut into the top or bottom later, but this is faster for a one off.

Next, making the box from this model

[enl_public]

Using the tool to make the case:

I began with the bottom (the steps for the top are the same, essentially). A new part is opened and the Derive operation is used. Most CAD systems will have something similar-- changes in the original will be reflected in the derived part(s). The first derived part is a rectangular block sized from the original profile. It would have been better if I had centered it, but I was lazy.

Then I added the caliper model (again using Derive) and positioned it where I want it.

The block and the caliper are two independent solids at this point. The caliper is embedded in the block, and will be used as a ‘toolbody’ to cut the block (the ‘base’) in a Combine operation.

You can see the hollow for the tool (open about 1/4" with extended cuts for the thumb grip and back side of the lock), but using this to make a case would result in a the caliper not fitting. Therefore, the walls are offset by to give clearance so the caliper will fit neatly without jamming. The clearance I used is 0.01" all around (to make it visible in the screen shot, I set it to 0.1").

The top of the box was done similarly. This is usable as-is, but features for hinges and a latch are very nice.

[enl_public]

Measuring for the latch:

The latch is a spring unit that is currently available from a variety of suppliers (McMaster, in this case). I could look the dimensions up on line, but it is easier to measure myself. The outside profile of each part is easy, since it is rectangular, and the overall depth (for both top and bottom combined) is measured with the parts snapped together. The screw hole positions are a different matter. I much prefer to have them done on the machine so the parts properly align top to bottom. Getting the center to center is one of the few places I prefer a figital (electronic) caliper to a vernier type.

Needed are two same-size balls a bit larger than the hole diameters. The digital caliper is used to measure one and is set to zero.

Now, the diameter of one ball will be subtracted from the measurement. The balls are held in the holes and the caliper is used to measure over them, getting the center-to-center distance, plus two ball radii. The measure ion the caliper subtracts the two radii (ball diameter), so the display shows the center-to-center.

It is actually rather awkward to take the measurement, since you need to hold the balls firmly seated while manipulating the caliper. For small parts like this, I usually just set the part and balls up in a vise (LIGHTLY) to hold everything in place.

Now, the pockets for the clasp halves are added to the box top and bottom. The pockets have their centerlines referenced to the box centerline (sie-to-side) and edge (top-to-bottom). For more involved setups, I would do this in a seperate template and bring it in the same way as the caliper was, but here, I just layed out centerlines and a rectangle. The holes were referenced to the centerlines of the rectangle and dimensioned to the proper spacing. Then, the rectangle was cut in and the holes ‘drilled’ with the hole tool (this cues the CAM system for the operation).

I also added a rebate at the back to position the hinges. The top was done the same way, but for the other clasp part.

Now that the models for the top and bottom are built, it is time to CAM

[enl_public]

I’m going to summarize the toolpath process rather than go into detail, for a couple reasons, primarily that it would be three times as long as what is already here to go into detail. The setup in the machine comes into play here, and it the first consideration. This includes what stock and where it will be fixtured.

In the interest of time and cost, I used prethicknessed stock (0.500" thick, give or take) and prepared it with two finish edges. These edges will not be touched by a tool. This lets me reuse the origin when changing pieces, lets me spend the time to square up only once, gives me some flexibility is fixturing method, and saves a lot of machining time (facing and border profiling are time sinks).

Note that the stock is oversized all to the left and back, and the origin is on top at the presized corner. Find it once, and the ACTUAL stock size doesn’t matter. Everything is relative to one point on the fixture.

The bar is set parallel to the bed travel and gives zero for y, and the round stop gives zero for x, with no chance of the material rocking and no way for it to be out of square (leading to rocking of the material). The material is dogged in from the rear and left for machining.

This leads to toolpaths that do the pocketing and only size on the left and rear:

The operations used are

The I actually duplicated the setup and operations for the case top, and only needed to select features. This a) is easy, and b) insures that the parameters will be the same (work it out once, then reuse it). Noth the last operation is the drill for the latch screw holes.

If you look carefully, you will see tabs around the perimeter. Lots of tabs. As the fixture squeezes the material to the reference bar, some strength is needed to keep the material from failing when the job nears the end. They come off easily-- about 5 seconds with a small saw and 15 seconds with a block plane. Also note that the cut doesn’t go to the bottom. It is about 0.020" above. This prevents cutting into the aluminum fixture plate. If I needed to go all of the way through, then a spacer could be used.

The parts right off the machine and test fit with the caliper:

And assembled:

The case will get a finish later, unless I make changes and recut it. There are a few things I might address, like no clearance to get a finger under the caliper. I wasn’t sure if I would need it, so I left it out. I think I might.

The total machining time for both parts was maybe 10min with a 1/8" two flute tool running at 10KRPM and 80IPM travel. The adaptive (trochoidal) strategy let me go with that speed at 1/8" axial DOC and 0.050 axial. Plowing the slot for the left and rear edges was done at 0.040" axial and the same travel. Probably I could have gone deeper, but the time samed isn’t worth the replacement cost of the cutter or damaging the machine. I really do not like slotting. It is hard on the tools. In this case, it let me not worry about hitting the fixture while holding the work securely.

I hope y’all have learned something. Happy New Year.

[WillAdams (William Adams (Carbide 3D))]

Very nice!

For folks who want to do something similar w/ Carbide Create there’s a tutorial on the wiki: https://www.shapeoko.com/wiki/index.php/Carbide_Create_Photo_Tracing#Machining_and_Finishing (and I added this as a Reference at the foot of that page)

[mikep]

Great tutorial! I’ve also done this using a photocopy of the tool (with a ruler in it so the canvas can be calibrated), and using that as a pattern/canvas in F360, and that worked pretty well too.

[tito (Bay Area and Sac, CA)]

Nice! – I especially liked the bit about using the ball bearings to find the centers of the mounting holes. Pretty ingenious. Thanks!