Why am I not able to put fillets all the way around?

[brendamat]

I have been making fillets in different groups so that I am allowed to create them. I am not sure what is the issue. 

Take a look:

https://www.screencast.com/t/rYAhAA45

[phlyx]

Sometimes Inventor gets 'confused' when there are too many complicated edge intersections.  It looks like this part should be symmetric (for the most part) but where the arrows point below the fillets on each side are not the same so something got out of whack from one side to the other.  If you do fillets one at a time (or pick the edges one at a time), usually when you click the one that it can't calculate all the preview fillets will disappear.  At least that would narrow down where the problem is occurring.

[brendamat]

Now that I was able to slect the last ones it is an error.

[Gabriel_Watson]

I think you'll need to share your file for others to try and see what's the issue here. Your recording does not provide the workflow to failure or a way to find how you intend to keep adding fillets.

You can try using the Analysis view mode to check if extrusions are not tangent to each other and if they connect well or not. This could be the issue why fillet won't solve in some areas.

Reference:
https://forums.autodesk.com/t5/inventor-forum/can-t-create-fillet/td-p/5475425

[brendamat]

Here is the file. 

[brendamat]

This is because there is a fillet in one of the sides and not in the other. It is going to be fillets on both sides. 

[brendamat]

I see the file I sent was not updated, but the problem on one fo the edges has been fixed. I will try to send the new file.

[brendamat]

But yes they are somehow not symetrical even when this is mirrored... 

[brendamat]

here is the newest file

[Gabriel_Watson]

If you remove every feature up to Extrusion6, you can see this area which is where I think the software gets confused, without space to create the fillet:

[brendamat]

so what would be the easiest thing to do here? to try to fix this cut after the mirror so that it follows the part profile? I have been trying different ways of doing it without getting it right. 

[Gabriel_Watson]

EDIT: these areas did not have side face edges matching the top faces properly, so I had an idea.... replace those side faces with a single one that would not clash with the seams of all edges on the top (and bottom).

1- create new boundary patch/face that merges the side faces through the bad area:

2- replace the side faces with the single boundary patch/face:

3- add fillet again.... and this worked here for the bad area, see file attached:

Similar thread I found later that shows a similar approach:
https://forums.autodesk.com/t5/inventor-forum/help-identical-corner-won-t-fillet/td-p/6382845

[johnsonshiue · Accepted solution]

Hi Brenda,

This is an interesting case. The fillet should work. However, the geometry isn't in ideal shape. First, some of the faces between edges are not tangentially continuous. This can lead to fillet failure due to imprecision. Second, some vertical edges may need to be filleted first. Please take a look at the attached image.

After you made these changes, the fillet should work.

Many thanks!

[brendamat]

So I modeled almost the whole piece again, using a different method for giving thickness to the part to the left. After I put the extra material in the face I mirrored the piece. What is very strange is that when I want to put the fillets, the fillets act completely different... They only way to manage is to give an extra fillet in the line on to top face to the right. Which ends up in a very bad looking fillet. 

When I try again it just keep getting worse... 

[brendamat]

hei, thank for this answer I am going to try it out now 🙂

[brendamat]

I am going to check it out, thanks. This is a picture of how the model should look: 

[brendamat]

It looks like a good solution but it seems like I will need to do the some to the whole model.

[brendamat]

It worked! 🙂 Thanks a lot, its been a journey trying to fix this problem. Have a nice day!

[brendamat]

And thanks a lot for this new knowledge. I have not use that tool before so this was a good thing to know 🙂 I was able to fix the problem fixing the first sketch. But this has been a whole journey to figure it out.

[Gabriel_Watson]

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@brendamat wrote:

It looks like a good solution but it seems like I will need to do the some to the whole model.

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Have you tried using my attached sample?
You only need to fix the problematic area, and 30 seconds later you are done. It allows you to fillet the whole part (I only applied the fillet to the area, but you can finish the entire part from my attached model).

I am attaching here again but with the fillet applied all around. This does not require any fixing of the sketch, and it is probably your fastest solution.