Model mill run-out for round

[EddyVE]

Using Creo 4.0 here ...

I have a 'handle type' part, that needs some edges rounded.

I have a problem with modelling the inner round because it has to stop 'halfway', where the red arrow is (see screenshot below).
If this part is produced on a milling machine, the round will of course not end 'abruptly' as shown below.

There will be some run-out of the radius mill.
How could I model this?

The inner round, I have now modelled as a sweep along a sketch (you can see the sketch as the blue line).

The mill run-out should look something like this:

Kind regards

[KenFarley]

For this kind of thing, to make the model look like what I'm going to make, I will add a revolved cut at end of the sweep. Revolve the shape of the cutter in the plane of the feature end. In addition to looking good, it's a pretty accurate representation of reality. A bit of work, but worth it.

[aputman]

You can draw a curve on the side of the handle and then create a round using the "Thru Curve" option.

[EddyVE]

@KenFarley  and @aputman , you guys gave me just the push in the right direction that I needed.
The solution (or one of the multiple possibilities) was fairly simple. The sweep along the sketch that I already had, just needed a little tweak.
I added an arc at the end of the sketch to provide the run-out path of the milling tool. Now why hadn't I thought of that!

The sweep mirrored:

[aputman]

That makes sense for something like a round-over bit on a router.  Glad you figured it out. 

[StephenW]

How are you going to specify that on the drawing? I can see what you did and I see why you did it, but explaining that part of the round seems problematic to me.

[EddyVE]

Stephen,
Fortunately here (as in most cases), the run-out is not critical. So in general I only specify the important dimensions and make a note that 'run-out is allowed'.
Something like this:

If more accurate specifications are needed, you basically need to know the dimensions of the tool. The radius mill in this case.

[EddyVE]

If you know dimension D1 (and R as specified), the minimum run-out radius is determined.
But so far I never needed to specify this detailed. 

[Patriot_1776]

Looking at the actual tool is what I recommended just so you know the tool's limitations, but you really don't need to know D1, only R.  You need to know D1 ONLY if you're programming the CNC toolpath, because then you know the centerline of the tool and offset accordingly.  But simply for CAD modeling, you don't need it.

[EddyVE]

Well, it depends on what level of detail you want in your model.
If you want it 100% accurate, you do need to know the pilot diameter (D1), because it will affect the minimal run-out radius.

R8 in the drawing below. A larger pilot diameter D1 will result in a larger radius (than 8 in my example).
Whether this is relevant in your design or not, was already a topic in previous posts. In my case (the part is 'just' a handle) it is not much relevant indeed.

[Patriot_1776]

One of the best things a CAD Monkey/Designer can do is think like the tools needed to create the part.  Be it CNC tools, or the mold the IM plastic or cast part are made from.  So, in this case, look at corner rounding tools on, say, Jergens, MSC, or Kennametal, and then think of the toolpath (sweep).  All you needed was that little lead-out curve.

[EddyVE · Accepted solution]

@StephenW @Patriot_1776 
Ok, let's go that extra mile and look at an actual tool to produce the round and make the model accordingly.

This is the matching sketch:

Note that the run-out (lead-out) radius can be larger than 3, but not smaller.

This is the sweep, modelled according the dimensions of the tool:

This is the result:

[StephenW]

Hahaha! I like it. I've used the term "Blend" to get something similar on drawing where I just needed a smooth transition out. 

But it's never a bad idea to understand the tools being used to do the job! 

Another option you possibly could have used is a variable radius, but honestly I think you developed a very good solution.

[EddyVE]

Small correction. My remark "Note that the run-out (lead-out) radius can be larger than 3, but not smaller."
Is not correct.
The run-out radius can even be as small as zero. It is the offset that can not be smaller than 3.
In the screenshot below: The 'red arrow R3' can be zero. The 'blue arrow 3' can not be smaller than 3, because it is half the pilot diameter of the radius tool.

Sketch changed so that run-out radius is 0.1 :