Fillet and draft frustration

[douglas.angle2]

This is my first Fusion 360 project.  I'm trying to make a pattern for sand casting.  I've been able to get the basic shape but need to add fillets and draft.  I've mostly been successful, except for a few locations where i get the "fillet/camfer cannot be created..." error, or the corresponding one for draft.  In this picture, for example, I can't seem to draft the blue face, even though I've been successful in the other 7 faces of the ribs.  I can't get fillets on one of the external edges or two of the internal ones.  I've watched tutorials, Youtube videos and searched this forum, without finding a solution that works for these particular parts. 

What I need help with is:

- draft on the blue face shown in the picture

- draft on the round piece out of the frame of the picture at top

- draft on the right end where there's a small red zone in the draft analysis

- 0.25 fillets on all exterior edges of the ribs

- 0.5 fillets where the ribs meet the body.

- less overall frustration with Fusion 360.  I'd settle for fixing the first 5 though.

Thank you for the help.

[wmhazzard]

It is best to do all fillets last unless absolutely necessary. I don't know where you copied and pasted the body 2 from but if you could delete the fillets there and draft first it might work. Also as it is now, there is some bad geometry that may be preventing the draft. 

 

[douglas.angle2]

Thank you for the reply.  I did see the "bad geometry", but the other 3 ribs drafted successfully with the same geometry.  In any case, I deleted all the fillets that intersected the face and was able to draft that one.  I still can't do the cylinder at the top.  I've tried deleting the fillets, but get an error when trying to delete some of them.  Still no progress on adding draft there.  Any other ideas?

[TrippyLighting]

My suggestion would be to start with a fully dimensioned and constrained sketch and stay away from splines until you have more experience with Fusion 360.

Then build on that.

Starting with something too complex in new software is invariably going to lead to frustrations.

[douglas.angle2]

My suggestion would be to start with a fully dimensioned and constrained sketch and stay away from splines until you have more experience with Fusion 360.

Then build on that.

Starting with something too complex in new software is invariably going to lead to frustrations.

I understand that there's some complexity in what I'm doing, but that's the nature of the part I need.  I've done lot's of 3D modelling for other simpler parts - I've just used wood and a tablesaw instead of software and a printer.  It's because this part is complex that I want to take advantage of 3D printing. 

Having said that, are you suggesting that it's not possible to fillet and/or add draft to the part once it's modelled this far?  Any insight as to why I can do that on one section, but not on an identical section elsewhere on the same part from the same sketch?

[TrippyLighting]

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@douglas.angle2 wrote:

Having said that, are you suggesting that it's not possible to fillet and/or add draft to the part once it's modelled this far?  Any insight as to why I can do that on one section, but not on an identical section elsewhere on the same part from the same sketch?

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No, I am saying that any solid design is based on a properly and fully dimensioned and constrained sketch.

Then you should draft, and then you should fillet. 

That will take some experimentation find the proper filleting strategy.

[douglas.angle2]

So I've reworked my sketch.  There's one gap in the constraints that I can't seem to fix, but otherwise constrained and dimensioned.  Now I'm having trouble with drafts. 

I've tried various permutations of the surfaces, but get one or more errors.  Can someone explain how to draft and exactly what's going on to generate the errors?

Curiously, I had trouble adding draft to the circular elements until I selected the inside face of the box as the pull direction, selected two-sided, set one side to 1deg and the other to zero, then repeated for the other side.  That doesn't make sense to me; why wouldn't it do both tapers at once? 

Once I do successfully draft and fillet the design, I need to generate cores, along with core prints as part of the pattern.  The cores and prints should be heavily tapered at the point where they meet the pattern.  So how do I create a taper/draft on one body using the pull plane from a different body?  I could do this for the bottom, where it's a flat surface by splitting the core at that point, tapering, then joining it back together.  However, the top surface isn't flat, so the actual start of the taper should follow the profile of the top of the pattern. 

[wmhazzard]

I got all of the surfaces to draft in the way that I would pull the pattern and it should be ready for fillets and core prints. You will probably need a follow board to get the bracket body to pull. 

To get the top surfaces to draft I went back and added a construction plane to draft from. For the inside circular features I used a negative taper angle in the extrude command. Go through the timeline and let me know if you have any questions. 

It is also advantageous to add the draft in your sketch so when you extrude there is no need to add draft.  

The core print is in yellow and is a basic extrusion with a combine cut from the main bodies. You will need to incorporate the inside of the bracket into the core. 

[wmhazzard]

Is this going to be full size or a scale model?

[douglas.angle2]

Thank you for your work. It's much appreciated. I would have replied earlier except that I've been studying what you did. I understand for the most part except:
- Why the need for construction planes? They are on the same plane as the interior face of the body, so why does a construction plane work but the face doesn't?
- I don't understand the last two operations ("delete face") where the excess was removed from the bottom of the core. I wasn't able to reproduce this - how did you do it?
- I'm left with one of my original questions - how to draft starting at the point where the core extends past the pattern. You added draft to the long edge of the core. I also need it on the short ends, but only where the core is exposed.

> Is this going to be full size or a scale model?
1/8 scale model.

> You will probably need a follow board to get the bracket body to pull.
> You will need to incorporate the inside of the bracket into the core.
I don't understand these two statements. Doesn't extending the core to the bracket eliminate the need for a follow board as the core prints will serve that function?

[wmhazzard]

- Why the need for construction planes? They are on the same plane as the interior face of the body, so why does a construction plane work but the face doesn't?

Because I did the draft before the interior cut out was made so those faces did not exist yet in the timeline hence the need for offset planes. 

- I don't understand the last two operations ("delete face") where the excess was removed from the bottom of the core. I wasn't able to reproduce this - how did you do it?

I just selected the inside faces and deleted them to eliminate the unneeded ends of the core print. 

- I'm left with one of my original questions - how to draft starting at the point where the core extends past the pattern. You added draft to the long edge of the core. I also need it on the short ends, but only where the core is exposed.

The short ends do have draft. The sketch for the core print was made by projecting the inside faces which already had draft applied. 

-I don't understand these two statements. Doesn't extending the core to the bracket eliminate the need for a follow board as the core prints will serve that function?

I wrote follow board before I finished the core so I probably should have deleted that since I think that the inside of the bracket can be part of the core. 

The draft tool basically uses a plane to start the draft angle from and can be either positive or negative  depending on the flip check box.

Lars has a short video on draft and there are others out there as well. 

https://www.youtube.com/watch?v=a6f6XAVEhu8