Taper a fillet?

[grahamUTKMN]

Hi,

I'm drawing a simple table top with radiused corners. I'd like the sides and front to have a top and bottom radius, but not the back.
I'm struggling to work out how to do that as shown in the picture. Is there a way to get the fillet to start where the blue circle is?

Thanks,

G

[davebYYPCU]

Not with a fillet, 

Three (5 would be more accurate) sketch Lofted surface and a Split Body does it.  Mirror for the other end.

Might help....

[grahamUTKMN]

Hi,

Thanks for the reply, but I don't know how to do that! 🙂

Is there a link or video showing me how do you know?

Thanks,

G

[davebYYPCU]

I can send my file in the morning.  Refer to my pic.

Knowing the corner fillet radius, create a sketch on vertical Offset Planes inset by radius value.

Project > Intersect - Body, in the sketches on those planes.  These will be purple section sketches.

Create the third plane as a horizontal offset plane.  Project > Intersect the body.  Add the corner fillet curve, dimensioned same as the offset plane distances.  Will turn black.

For top and bottom fillets in one go.
Go to Surface Tab, start a Loft.  
Profile 1, is the vertical purple straight line on the back wall of the block.  

Profile 2, is the top fillet purple curve + vertical line + bottom fillet purple curve. (Front of pic)

Select the black centreline Rail curve as the Centreline Rail.

Ok.

Modify > Split Body, cut the block using the surface lofted Body, as the cutter, say Ok.

Remove the offcut with Remove Tool.

Go to the Solid tab,

Create > Mirror - set feature.  Select the Loft and Split Body icons, off the Timeline.

Select the block vertical centre origin plane, (or Midplane), ok.  

Remove that offcut.

Might help…..

[grahamUTKMN]

Thanks again for the reply, I've never done a loft before, I'm very confused how to do it.

I've tried watching a couple of videos, but still stuck 😞

G

[grahamUTKMN]

I've tried to follow your steps, but I've done something wrong somewhere...

G

 

[davebYYPCU]

Ok you’re nearly there, 

I forgot to tell you that I started with a square corner, no vertical fillet.  That’s why my horizontal sketch needed the black curve added to the corner.

Before you make the Loft, hide the solid block, 

Before making the selections, (Untick chain select)

you do them in the same order I said, you will see Fusion start making the cutter body, when you select the top curve, and you add the vertical line, and bottom curve for profile 2.

Change the Rail section to Centreline, (2nd type icon)

Might help…..

[davebYYPCU]

Attached my file, Mirror features worked as expected.

[grahamUTKMN]

Thank you for your help! I think I'm nearly there now.

I've done the loft, but when I try to split the body I get a compute failed error.

I have attached my file.

Thanks,

G

[davebYYPCU]

Works as expected.

Split Body > select plate body, and then select the cutter body, (it's embedded) by clicking on the body name in the browser.do not click extend cutter body.

Not sure how you can make it fail.  I checked the Loft, after posting this pic, and you will get a better more tangential result, if you edit the Loft, delete the current Rail, change to Centre Line rail type, and reselect the rail curve.  Much better.

Might help...

[grahamUTKMN]

Hi,

Possibly me doing the split wrong?

I am doing Split Body
Selecting Body 1 from the Browser as the Body to Split

Then selecting Body 3 as the splitting tool from the Browser

 

OK
And I get Compute failed:

 

Have I done anything wrong here?

Thanks,

G

 

[davebYYPCU]

Nope, same as I did, one thing though, the fillet edge lines are in the last pic, as if it did perform, nah disregard, that is the cutter body showing.

However, done it for you, and sending back.

[grahamUTKMN]

Thank you, I just tried altering the centerline on the loft and then gave it one more go, and then it worked!

My model is now correct.

However, now when I try and produce a 2D drawing, it does one of the corners wrong. Maybe something is going wrong in the mirror command. It works in the model, but not the drawing.

 

 

 

 

G

[davebYYPCU]

Ok, great.  I don’t think I ever tried a split body, with an ordinary Loft rail, you had me going there a bit.

I’ll presume, you have cut and Removed the offcuts, and the cutter, only one body left in the browser before going to Drawings.  Sketches not visible?

Sorry, I don’t think I have eve made a “Drawing” in Fusion.  I have zero experience there.

See if @ClintBrown3D can help out.

Might help…..

[sanjay_jayabal]

Hi,

Is something like this what you are looking to achieve?  If so, you can do this with 2 fillets.

Best regards,

Sanjay Jayabal.

[davebYYPCU]

No, we have the correct geometry sorted out, now progressing to Drawings is inaccurate.

Might help….

[tnomura-jt]

Variable fillets?

[jbdennison]

Thank you for this reply.  This was just what I needed for a related question.