Trouble Filleting A Part

[Anonymous]

Ok I took your advice and started over.  Constrained the sh*t out of everything and when I say everything I'm not kidding, going so far as duct taping my laptop to my desk left to right, up and down, my dog too.

Results are worse now than what I had before.  For the time being my issue isn't "shelling" the part, yet, but now it won't allow me to put a .75 fillet on both sides of a 1.5" wide square tube.  This is maddening!  

I read your previous suggested reading.  Didn't help much.  The tip about being able to switch the work plane view was handy, but outside of that no help toward my issues, which was originally "shelling" but has now morphed into not being able to fillet what looks like a simple filleting task.

A tip to Inventor's powers that be:  How about giving the user the ability to simply highlight the sketch, right click & get a menu with a "constrain" or "dimension" command that can then be left clicked and viola, done!  Is there a reason this can't be done?  I think not.  It's infuriating struggling to "fully constrain" a sketch while seeing the number of measurements Inventor is asking for down in the bottom right of the screen.  If it knows it needs those two measurements, it also knows where those measurements are that it's looking for.  Is it me?  Am I missing some other visual que telling where those measurements are that it needs?  Without visual ques it's a maddening guessing game of hide & seek!  What's more, even after the sketch goes blue in color indicating all is well you can still get the prompt at the bottom right of the screen saying it needs 1 more dimension!  This is infuriating as often times there are more than enough dimensions all over the screen yet Inventor is asking for some oddball measurement but not indicating where it needs it!  

So a simple highlighting of the sketch, right click and left click on  "constrain" or "dimension" solves this problem and makes this miserable software just a little less miserable to work with.

Attached is the new attempt.  Can't put a .75" fillet on the 4 edges running the length of the loft.

Another moronic Inventor function is to get the idiot box that pops into view telling the user there's a problem with the action the user is trying to initiate.  It goes on to say a bunch of nonsense that only a PhD user would understand.  Really stupid.  In fact, colossally stupid.  Does anyone inside Inventor's management have any clue how irritating it is get an error message without Inventor explaining in laymen's terms?  

I also noted in your helpful hints link that you mentioned NOT using the "mirror" command.  I've been told by others NOT to use it either.  Pretty clear the reason not to use it is due to shoddy software programming which there is no excuse for when paying $7,000.00 for software that has been on the market as long as this one has.  I don't have the $7,000 version but I can tell you I won't be buying it after seeing how miserable this version is to work with.

Anyway, enough of my rant.  It had to be said.   

[JDMather]

Exit out of that sketch.

Right click on the sketch in the browser and unselect Dimension Display.

Start a new sketch on the front plane.

Project Geometry the top and bottom lines from Sketch 1 Create a rectangle from the upper left corner down to the bottom line as shown to the left.  Add the dimension.  It should be constrained with one dimension.  Add second rectangle approximately as shown.

Create Rectangle as shown.   Note that I always turn on Visibility of the Origin Center Point.

Note that I have exaggerated the angled line to the midpoint of the vertical line in the rectangle.

[JDMather]

Add horizontal constraint to the angled line and the dimensions as shown.

[JDMather]

Right click on Sketch2 in the browser and turn off Visibility.

Start a new sketch on the right side plane.

Project Geometry the top and bottom lines of Sketch1.

Create a Rectangle as shown - picking the projected point at the top first.

Then drag the point shown red at the bottom of the rectangle to the bottom projected piont from Sketch1

[JDMather]

Finish Sketch3 as shown.

[JDMather]

I decided to add this 8" construction line to Sketch3.

[Anonymous]

Ok, working well now...

[JDMather]

Create a workplane at then end of the 8" line by selecting the line and the endpoint.

Start a new sketch on this workplane.

Project Geometry the lower left corner of Sketch1 (shown red) to the new workplane.

Create the rectangle as shown.

Add and Equal constraint (=) to a vertical and horizontal sides of the rectangle.

[JDMather]

Extrude Sketch1

and then Extrude Sketch 3 to cut the angle.  (This could have been done as one Extrusion from the right side plane.)

[JDMather]

Loft from the angled face of the part (note that no sketch is needed) to Sketch4 as shown.

[JDMather]

I have to go for now, but just for fun -

Edit the Loft feature and on the Conditions tab of Loft, set the Condition for the Edges selection set to Tangent.

- back tomorrow.

[Anonymous]

Ok.  Here's where it's at now.  I'm going to have to stop for now and come back to it tomorrow.

Thank you for talking me off the ledge.  I might get some sleep tonight...

[JDMather]

Delete that angle dimension - not needed.

Drag the endpoint of that bottom line down and back up and it should snap to the projected point at the bottom of Sketch1.

[Anonymous]

Ok I tried the "tangent" setting in the loft condition.  Interesting, but I'm not happy with the shape it created.  The radius is much too big and too far forward.  I prefer the steeper angle of the loft with a much smaller radius without the "tangent" condition being applied.  

I can see how using the "tangent" setting is a great way to make sure everything's symmetrically equal though.  

[Anonymous]

Ok, the inability to fillet has raised its ugly head again.  

[JDMather]

To me it seems like you have the radii on the Fillets 1 and 2 backwards (concave greater than convex), but in any case, these fillets are causing some strange anomaly on the lofted faces.

The "solution" is pretty easy though - Delete Face the entire faces on the sides as shown in image.

Then select Patch and patch the face loops.

Stitch back together into a solid and you should now be able to fillet.

Oops, I found at least part of the problem -

Move Extrusion 3 up before Fillet 1 and 2.

[JDMather]

Whoa, Sketch5 is all wrong (dependent Projected Loop) and not even needed.

The sketch had already been created as Sketch2 which never got used.

Simply turn the Visibility of Sketch2 back on and use for Extrusion3 (before Fillets 1 and 2).

Didn't you wonder why we created Sketch2?

[Anonymous]

I knew that sketch was already done, however, I didn't know how to get back to it to be able to utilize it.  I didn't know all I had to do was click the "visibility" to get it to become usable again.  So I did (after deleting sketch 5 and what happened wasn't pretty.  The problem was two fold:  First, as soon as I deleted sketch 5 the cylinder moved across the screen way out of position.  Second, when I went to extrude that portion of sketch 2 it was in the wrong direction causing it to be in the "cut" direction so it wouldn't extrude.

I haven't yet monkey'd with the faces of the loft (as you can see) but am including the drawing as it is now to give you an idea of where I'm heading overall.  I'm not sure if filleting those edges now is the right thing to do or should wait till after I connect the cylinder to the adjacent fact between fillets 8 & 9?

[JDMather]

---

@Anonymous wrote:

  Second, when I went to extrude that portion of sketch 2 it was in the wrong direction causing it to be in the "cut" direction so it wouldn't extrude.

---

Simply flip the direction in the Extrude dialog box and set to Join rather than Cut.

This is pretty basic stuff.

I recommend that you go through these

http://inventortrenches.blogspot.com/p/inventor-tutorials.html

[Anonymous]

I figured it out on my own, but thanks for the link.

I tried to figure out how to use the "delet face" & "stitch" commands but couldn't figure out how to "stitch" everything together after the faces were deleted.  You'll see I only deleted the faces on one side as the other side I'm able to fillet both the top & bottom edges without trouble.

Can you advise me on how to "stitch" the deleted faces back together?

So now that you can see the direction I'm heading in what do you recommend as a solution to connecting the cylinder to the side of the long draft where it meets the radius near the bottom?

[JDMather]

You have not followed my instructions - so for me to continue - we will have to start over. Are you willing to do that?

If so, drag the red End of Part marker up the feature tree to just below Loft1.

Right click on the red EOP marker and select Delete all below EOP.