Fillets operating in reverse

simon_9

I am trying to fillet between two objects - in this case a tube and the plate to which it is attached and the fillet is going down into the plate rather than merging the tube and plate on the face I want...

I must be doing something wrong but I have no clue what it might be - any help out there please?

And since a picture is better than a thousand words, hopefully the screen shot shows what I have at the moment.

Simon

pete_yodis

Potentially the tube and the plate are two separate bodies.  The fillet is not a "weld" operation.  You need to do a Boolean operation on them first (add the bodies together) and then fillet if that is indeed the case...

pete_yodis

Potentially the tube and the plate are two separate bodies.  The fillet is not a "weld" operation.  You need to do a Boolean operation on them first (add the bodies together) and then fillet if that is indeed the case...

simon_9

Hum - well yes I think you have answered the question - however I have spent the last 30 minutes trying to do a boolean on the pieces of tube at an angle and the extrusion and I cannot get a merge to happen.
But thanks, I am sure your answer is right, I just need to join the two bodies into one.

Ben_

Then the parts may be separated by a tiny bit and not allowing for boolean. Try and extrude the ends of the tubes to the other part or move them a smidge closer.

andrew_troup

Even parts which are touching cannot be joined, if (at ANY point) there is zero thickness. 
Simplest cases: Imagine two perfect cubes whose diagonals are aligned, with corners touching. Or a round rod resting on a flat part. In such cases, a boolean merge is not viable.
Two regions of a solid cannot be connected by a single edge.

Although it's a kludge, a simple way to force contact might be to use "Move Face" on the appropriate faces of your tubes, and/or main body. It's generally better to edit the original geometrical basis, though, particularly if there are any functional or manufacturing implications.

3dcad

Can you change the extrude of the tubes to 'Add' instead of 'New'? This way you don't need to use boolean to combine.

simon_9

Thanks for all of the suggestions - the initial problem was as suggested by Pete_Yodis, that I had more than one part.
To get everything glued together I eventually rolled back a number of steps and extruded the base plate up into the circular array of tubes and then later removed the holes now blanking off the tubes - I am sure that there is a better way but this worked in the end and that's what the objective was!

Now trying to glue the last two parts together - something I will take more care with in the future, its a pain having to rework like this when I could have done it better to start with.....However having the ability to roll back easily helps enormously.

Regards to all,
Simon

pete_yodis

@Simon, you could have edited the feature that created the body(ies) as @3dcad mentioned and selected 'Add' as he mentioned.  This would "merge" the geometry together without needing to do a separate body combine/add command (Boolean operation).