Keep getting a 'pcurve' error message when creating a fillet.

[0806056]

Hi all,

I'm having difficulties creating a very simple design.

I have sketched my shape and extruded everything. To finalise I want to give all corners fillets. But for some reason Fusion won't let me create a fillet on a specific corner. I keep getting the error message: Error: cannot add a pcurve to this entity. 
The opposite corner, which is exactly the same does not not give me an error and just creates the fillet.

I have tried googling it, but can't find any information on 'pcurve'. Its very weird behaviour because all the other corners have no problems.

Does anyone know how to solve this issue? Or guide me to what I'm doing wrong.

I have attached the fusion file

Thanks in advance!

[TheCADWhisperer]

@0806056 

Are you sure that you want to use Splines for the curve rather than simple arcs?

I would fully define my sketches.

[0806056]

thank you for your reply. 

Does it matter for this fillet error? I'm fairly new to Fusion and Splines got me the result I needed. I couldn't manage with arcs.

[TheCADWhisperer]

@0806056 

Let me see what I can come up with.

Check back...

[laughingcreek]

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@0806056 wrote:...Does it matter for this fillet error? ...

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yes, it does.  the underlying math involved for splines is vastly more complex than for arcs.  frequently in circumstances like this, fillet will struggle/fail with surfaces created from splines but do fine when arcs are used.

also, your part won't have a consistent thickness the way you are doing it.  better would be to create a surface, cut out the interior shapes, and then thicken.  that will insure a consistent thickness.  I would do an example but I suspect @TheCADWhisperer will be posting one soon that uses either the thicken workflow, or possibly a Sheetmetal one.

[TheCADWhisperer · Accepted solution]

@0806056 

There are many ways to do this...

I made a change to the outer Fillets 10+8=18, but you can change back to 10 if desired.

Observe that the sketches are fully defined and relatively simple.

If I get time, I will demonstrate a completely different technique that is probably closer to how you would model as a beginner.

[0806056]

Thanks so much!

I'm having a look and trying to figure out how you have done it.

How did you draw the 'S-curve'? What method did you use and how did you calculate the Radius?

Also a little update, I started from scratch again using the exact same methods I used before (control point spline) and now Fusion would make all the fillets properly. Seems I ran into a bug. Anyway I will dive into the suggestions and figure out how to move forward.

[johnsonshiue · Accepted solution]

Hi! This is a limitation. There is a very short edge connected to the vertical edge. In order to round the corner, the fillet face will need to be broken into multiple pieces. Removing the short edge will make the fillet work.

Many thanks!

[TheCADWhisperer]

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@0806056 wrote:

How did you draw the 'S-curve'? What method did you use and how did you calculate the Radius?

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Two 3-point arcs connected with Tangent line.

For the radii I set close to your spline with integer radii.

Check back for another technique.

[TheCADWhisperer · Accepted solution]

@0806056 

Here is a different technique.  There is a subtle but significant difference in the Fillets compared to Thicken.

Also, I changed the outside filets to 10+14.65=24.65

[JamieGilchrist · Accepted solution]

One other way for the base shape,  I did it using Thin Extrude, so you don't have to create a closed profile.  In all the provided examples, you'll end up with a. vastly simplified timeline, making troubleshooting problems, when they occur, much easier to resolve.