Radius all points

[difalkner]

What is the best way to radius all points to 0.065"?  Now, what is the easiest way to radius all points to 0.065"?  They aren't always the same solution...

I have been doing them with 3-Point arc but that's more a guess.  After I draw it then I have to see if I actually got it right and if not then I delete it and try again - painstaking long process. 

For this application I can't use filet so I need to draw in the radius.  I only circled a few but I need to radius all points.  I've attached the file if that will help.

Thanks!

David

[TrippyLighting]

---

@difalkner wrote:

 They aren't always the same solution...

---

What exactly do you mean with that ?

[ToddHarris7556]

In general, I'd say that the filleting is probably BEST done and EASIEST at the feature level. i.e. leave the corners in the sketch sharp, then extrude/cut/whatever, then apply your fillets last using the FILLET feature. There are actually multiple reasons for this.... but this isn't what you asked. 

I would suggest the next-best approach would absolutely be to use fillets in the sketch. Use an geometric EQUAL constraint, and control exactly one of them with a parameter. But it sounds like you have reasons for not doing it that way. 

Using 3-point arcs manually runs the risk of missing some inferred tangent constraint, inadvertently dragging something... in general sounds like a ton of work, with a high risk of breaking something. If you absolutely HAD to do it this way, I would probably suggest turning all of your master sketch geometry into construction lines, and sketching right on top of them. This way you could easily infer the tangent constraints as you go, and go back and set all the radii equal afterwards. I wouldn't think this is the best or easiest way, however. 

[ToddHarris7556]

FWIW.... I was wondering the same as @TrippyLighting... in my experience, taking 'shortcuts' typically might be easier in the (very) short run, but result in significantly more work (harder) in the long-run. So.... the 'best' way is almost often what I view as 'the easiest overall' solution. <shrug> 

[HughesTooling]

You could try window select for the top view the switch to a side view and window select with the Ctrl key down to unselect the top and bottom edges. This might be difficult if the part and pocket are not very thick, just temporarily increase the thickness, add the fillets then reset to the correct thickness.

Mark

[HughesTooling]

@difalkner Didn't notice you'd attached the model. Here it is filleted, because of the shape unselecting some edges needed to be clicked on individually with the Ctrl key pressed but it was still only one window selection from the top then 4 from the side with Ctrl pressed then 3 clicks on the lines still selected.

Mark

[HughesTooling]

Here's a screencast using your file. 

Mark

[difalkner]

Thanks, guys.  What I mean by best and easiest not always being the same is best defined by a couple of illustrations:

1) I want a nice, hand rubbed, French polish shellac finish on a piece of furniture or guitar but I don't want to go through all the labor and time to do it that way.  So I grab a can of spray Shellac and spray that on and then do a little rubbing so it doesn't look like it came out of a rattle can.  The hand rubbed and labor intensive French polish finish is the best way to achieve that look but it isn't the easiest.  The rattle can is the easiest but it won't look as good. 

2) I need to rip a board for a piece of furniture and am shooting for a hand-built piece.  So I decide to grab a rip saw and cut the board by hand.  15 minutes later I have a board with a mediocre cut that now needs to be straightened up with a plane.  Or I can cut it in 5 seconds on the table saw and have a perfectly straight line and still claim hand-built for the rest of the piece.  The table saw is both the easiest and best way to do this cut.

So... on to the reason I don't want to use fillet (and yes, I see I mistyped it in my original post - sorry).  The pieces off to the right are derived from the pockets in the main board by using offset, reducing the size by 0.0075" and then extruding out to 0.150" to become inserts for the pockets.  The main board is Walnut and the inserts are Maple. 

Because I can't cut square inside corners with a round bit I need to radius everything for a drop in fit.  I'll be cutting these with a 1/8" bit, hence the need for a radius of about 0.065".  So I figured if my drawing had the radius in it and I used offset to create the inserts then everything would fit.  If I use fillet for the pockets, which is easily done, then my inserts will still have sharp corners and points if I create them by using offset.

So maybe I should be asking if there's a way to create a new body after the fillet is applied so that the insert will match and drop in the pocket.  Is that doable?

Either way I need to be able to do these so the inserts fit with minimal tweaking.  If I was going to make just one of these I would just leave the inside corners and points as the 1/8" bit left them and clean them up by hand to fit the inserts.  But I'll be making several of these and don't want to do that much hand work.  It'll take too long and my back and eyes would complain!  LOL!

Hope this helps - thanks again!

David

[HughesTooling]

The quickest way will be to model size for size and offset in the machining op in the CAM workspace. You might even make the inserts as a single part to make selection easier. Also you could make them as a single block glue in place then machine away after.

Screencast should give you an idea of what I mean. As I've used a combine cut after creating the pockets and fillets the inserts will always match.

Mark

[HughesTooling]

Take a look at the attached file, Hint Section is active. I've added a couple of press\pulls, one to increase the depth of the inserts and one to add an offset. I selected the offset in a similar way to how I selected edges for the fillets in the screencast in post #7.

Mark

[etfrench · Accepted solution]

The pockets don't need to be modeled for 2D machining. 

It's a simple operation to fillet the geometry in the sketch, then create the CAM toolpaths:

Instead of using the Contour toolpath for the inserts, a Pocket would be easier. 

[ToddHarris7556]

I would very much use the approach that @HughesTooling showed. I wouldn't have thought of @etfrench's pocketing idea, but it's cool, too.  

In terms of 'easiest'/'best', personally I would say key points include:

• I'd definitely cut both parts off the same geometry. i.e. don't copy a second sketch off to the side. Too many chances to introduce error.
• Building on that, the 'combine/subtract' method pretty much guarantees that you haven't missed a selection anywhere. The solids will match.
• selecting all the vertical edges using Marks' method ensures that both the male and female parts will be properly filleted.  
• when we work with imported sketches like this, we try to leave the sketch well enough alone.... filleting in the sketch it's too easy to accidentally move something, and too much work to ground/project/retrace. Turn it into a solid fast, and work from there, IMO
• as Mark offered.... standard best practice in our shop would be to model for size, machine to fit. i.e. model both contours the same , then use 'Stock to Leave' in CAM to control how precise the fit is. The only time we'd actually model in clearance is when it's actually required for functional reasons. 

[HughesTooling]

This thread might be of interest if you ever need to produce sharp corners.

V-Carve Inlay Anyone?

Mark

[chrisplyler]

I would...

1. Create a Component for the base.

2. Model the base.

3. Extrude cut all the pockets down into the base with sharp corners.

4. Modify>Fillet all those sharp corners.

5. Create a new Component for the inlays.

6. Construct an Offset Plane up above the base a little ways.

6. Sketch the inlays by projecting the already filleted pockets, and offsetting those projected shapes inwards a couple of thousandths.

7. Extrude the thickness of the inlays.

8. With one Rigid Joint, place the inlays down into the pockets.

Since the inlays are a couple thousandths smaller all the way around than the pockets are, they should easily assemble with a bit of wood glue and tapping then gently into the pockets with a rubber mallet.

[difalkner]

Wow!  You guys have some seriously good skills at this - thank you so much!

I didn't see the post by @etfrench until today and the others are, I'm afraid, a bit beyond my understanding of the program.  Some of the videos wouldn't go full screen and I can't quite tell what's happening.  Some parts of each make sense to me but some don't and since I needed to get the plaque finished and out to the customer I did it the hard way - manually radiused each point.  And yes, it took a while.  And the inserts didn't fit without some hand work.  They were close but not a drop-in by any means.

So fast forward to today and I have another order for a slightly different plaque but basically the same.  Instead of a Command Chief this one will be an SFC Stripe (I wasn't in the Air Force so no idea what either is...).  This one doesn't have the stars and is slightly smaller.

But I saw the post by @etfrench and radiused every point to 0.65" in a matter of about two minutes where the other one took hours. 

I still need to work on the inserts but I may try a test with cutting the inserts with Pocket instead of Contour.

Here's the finished Command Chief plaque.  The last shot is the plaque in front of the guitar I just finished building.

Thanks so much, guys!  Sorry it took a while to get back with y'all.

David

[TrippyLighting]

Very nice results indeed!

These threads I find very satisfactory, but this is what Fusion 360 is really about. Making things!

I know that @jeff_strater enjoys this stuff as well.

[etfrench]

Well done. Both the guitar and plaque look great.