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FreeCAD and fixturing- How to model holes in the side of a cylinder.

 ·  ☕ 7 min read  ·  ✍️ Cj

Always need more tooling

I suddenly find myself in need of holding an 1-3/4" diameter threading die in the lathe. I’ve got some parts that need a 3/4-20 thread put on them and single point threading is pretty slow when tight tolerances are not necessary. I would have been content to just buy another die holder but what do you know? Every one I could find only holds threading dies with max OD of 1.5". Well I guess it’s time to warm up the CAD system and scrounge around for an unclaimed chunk of steel stock.

The only part I purchased for the project; a #3 Morse taper shank with a 5/8-16 end:

collecting parts

Starting the design

There are going to be a lot of holes drilled through the side of the main cylinder here, a task which seems to offer a lot of frustration for newcomers to FreeCAD. I’m going to offer what I consider the quickest, most parametric solution I know of. This certainly isn’t the only solution you’ll find to the problem, but it’s been very reliable to edit after-the-fact and for me, it is a way that makes sense coming from a mostly Solidworks background.

This short tutorial assumes you have some basic knowledge of FreeCAD, the Part Design workbench, and the Sketcher.

A note about versions

The version of FreeCAD I’m using for this tutorial is v0.19. I highly recommend anyone still using 0.18 to go ahead and make the upgrade. It’s pretty stable, and there have been tremendous improvements especially in the area of the TechDraw workbench.

Note: Models made in one version should work fine with the newer/older version. The same is not true of prints made in the TechDraw workbench.

Getting started

Coming from Solidworks I tend to think of nearly every solid body and part feature as starting from a sketch; one that was either extruded or cut into a previous extrusion. So that’s how I like to begin all my parts, even though some prefer generating basic primitives (cube, cylinder, etc).

Througout this tutorial you may see me slip up and refer to some operations as an ‘extrusion’ or an ‘extruded cut’. This is what Solidworks calls it. In FreeCAD we would call these operations ‘Padding’ and ‘Pocketing’ respectively.

A sketch with a single circle, sized to 2"

basic cylinder sketch

Pad the sketch 2.5"

cylinder sketch extrusion

Select the end face of the cylinder, create a sketch, make another circle and size 2.5". Extrude 0.8":

Concentric cylinders complete

You’ll need to change all these dimensions if you’re using a different size Die of course.

  • This die is 1-3/4" diameter, and a little bit over 1/2" thick. I’m going to bore this 1.755" for clearance to fit the die in.
  • The center hole is 1". It could be made bigger if you need clearance for a 1" thread.
  • The smallest rear hole is 0.565", for threading 5/8-16. An odd thread choice indeed.

Helpful tool I only just discovered: Right click in the Combo view on the ‘Body’. Click ‘Appearance’. Now adjust the transparancy. Very helpful when working on interior part features

Center steps complete transparant

So here I have extruded two sketches into my stepped cylinder, a bore for the threading die, and the threaded mount in the back. There will be several features needed in the sides of this cylinder.

  • 4 Holes for setscrews to secure the Die in place.
  • 1 Large cross-hole to allow chips to clear the workpiece.
  • a partial counterbore to allow for a setscrew to secure the holder to the Morse shank.

Construction geometry is the key

It’s possible to construct other cylinders and use boolean operations to make your holes, but I find this method cumbersome to reference features to one another.

The method I use is to build a sketch, extrude it, then use that surface to build my second sketch on for the actual cuts into the cylinder.

Construction sketch

So here I make a sketch on the front face of the holder. Size it so that the upper surface is the same height as the existing part. Width is less important, but keep it centered around the part axis:

construction sketch

And that’s padded (to any distance) and makes a face from which we can build our second sketch

construction face selected
construction sketch padded

It might seem odd to pad out this sketch, but a solid geometry is required for future sketches to reference properly.

Use the ‘Create an edge linked to an external geometry’ tool to import the lower edge of our construction geometry, and reference the location of our holes off of it.
cross hole sketch

I have applied our cross hole (for allowing chips to fall out), and a pocket half-way out the back for a key-screw. These are done as two seperate sketches since one is pocket ‘through all’ and one has a limited depth (0.45")

Now simply create a sketch on the side of our construction geometry, and pocket it away:

sketch to remove geometry
construction geometry removed
So now our construction pad is cut away, cannot be seen, and will have no influence on any future geometry we add to the part. Yet it’s presence is still recorded and references to this geometry still exist.

There are 4 dimples in the threading die for setscrews. We will use all 4, 10-32 screws in this case.

Create a new construction geometry on the front of the part, and pocket a single hole:

sketching for set screws

No need to make 2 sketches on each side, we’ll just apply a Polar-Plot around our center axis.

polar plotting setscrews

Clean up our second construction pad, add a few chamfers. It’s looking pretty good:

perspective view

Make a print in the TechDraw workbench and it’s off to the lathe.

Click the image for a PDF version

schematic screenshot

The machining

Starting with an old chunk of mild steel. Drill the center, bore the pocket for the threading die.

boring the die holder

Turn down the outside and chamfer the edges

turning the outside
5/8-16 is a bit of a strange thread you won’t find on the drill-tap charts. It can be found in Machinery’s Handbook of course. No clue who designed that Morse shank to have that thread. I certainly don’t have a tap for it, so we’re single pointing the thread.

Single point ID threading

single point id thread

I need to index this on 4 sides for drilling the set-screw holes. It’s too big for the 5C collet block, so I threaded a piece of shafting and mounted the die-holder to that.

So next we start drilling and tapping

tapping sides

Arg, it’s wobbling again!

So it turns out just threading that shaft to hold the die-holder for drilling isn’t quite tight enough. It’s twisting as I drill the large cross hole. What I should have done is threaded the shafting further back, then perhaps make a nut that can be jammed up against the holder to keep it from twisting.

Taking it slow and added a finger clamp for now

added finger clamp

Installing the shank

Threaded mount for a threading-die holder won’t do as-is. When the lathe is reversed to back the Die out, it’s just as likely to unscrew itself from it’s mount!
So what I’ve done here is counterbore down to the surface of the shank, drilled right on the parting line between the two parts, and tapped it 10-32 for a cap screw to keep the holder from un-screwing itself. It’s also removable if I want to make more fixturing for this shank in the future.

Tap carefully. The shank isn’t hardened steel but it is much tougher cutting than the mild-steel die holder. Both the drill and the tap wanted to wander off center. Don’t break on me now tap!
counterbore for screw pin
mount complete

Finished! In the tailstock, ready to work.



In case anybody wants them, here’s the FreeCAD file and a PDF schematic
FreeCAD files for 1.75" die holder
PDF schematic print of die holder

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