Overlapping Flanges Don't Mitre Inventor 2011 1

[cjjatpuresilica]

Hi,

Can anyone please help me overcome the inability of the flanges to mitre in the corners.

I have tried numerous models, including repairing Inventor, all to no avail.

Any help would be greatly appreciated.

Thank you.

cjj

 

[rollupswx]

I noticed that your first sketch is not constrained or making use of obvious symmetry about the origin.

http://home.pct.edu/~jmather/skillsusa university.pdf

...and I would probably model "as folded" rather than folding up from a flat (let Inventor figure out the flat).

....and do you really want a bend in the middle of what looks to me could be a simple planar face (resulting in this split)? (see attached)

 

[cjjatpuresilica]

Dear rollupswx,

Thank you once again for coming to my aid.

I am somewhat puzzled by your comment vis-a-vis my face sketch not being constrained.

Although it looks a simple model it is in fact quite complex, hence the reason I have folded from the flat. I will however try extruding from a single face, as per your kind suggestion, to start off with and see how that works.

But, without wishing to appear ungrateful, non of your observations seem to account for the failure of the flanges to mitre in the corners, which is my prime concern.

Thank you.

cjj

 

[rollupswx]

Look at where the origin is and where the center of your sketch is.
Wouldn't it be obvious to place it (automatic coincident constraint) at the origin as suggested in that document I linked earlier (same BORN Technique in MDT).

 

[rollupswx]

Inventor is telling you the sketch is unconstrained.
First thing the guy out on the shop floor does is set up absolute datums so he knows how any changes will effect the design. As your is I can drag the sketch anywhere around the screen. Not predictable. Same as in MDT.

 

[rollupswx]

Notice that when I constrain to the origin the geometry changes to a dark color - visually letting you know that it is fully constrained and needs no more dimension/constraints.

And don't change the properties of your construction geometry - Inventor will do that for you. Simply toggle to construction (see attached). If you insist on doing the extra work of changing properties (ACAD users like to change colors - you will quickly get used to it if you let Inventor do it's defaults) at least DON'T use Pink (magenta) as that indicates SICK geometry by default in Inventor. Use anything but pink.

 

[rollupswx]

I've got to run just now - I come back and answer the solution to the Flange Miter in a bit.

 

[cjjatpuresilica]

Dear rollupswx,

I appreciate that I am asking an awful lot but is it possible for you to please modify my file as it should be, that way I can compare it to my original to see what I am doing wrong.

In addition how do I set up the default styles for construction etc. I simply cannot cope with the horribly thick lines that Inventor seems to use as default?

I am most grateful, for I have been struggling with this for nearly 3 weeks now.

My kind regards and sincere thanks,

cjj

 

[rollupswx]

You must not have looked at the image I posted.
When you change a line or circle to construction Inventor automatically makes it much thinner (less than half the thickness of an object line) and dashed.

When I get a chance I'll show how to fix your part, and then how I would have done it from scratch.

 

[rollupswx]

This image shows Inventor Object lineweight, Iventor's Construction lineweight and YOUR construction lineweight.
If anything, yours looks slightly thicker than Inventors "horribly thick" construction lines.

Quite frankly in my experience teaching someone who exhibits what I see as a glaring lack of geometric observation I expect a long road ahead. We'll see how it goes. Stick with me.

 

[rollupswx]

If (big if) I was going to model from flat - here is how I would do those corners.

 

[rollupswx]

But of course, modeling from flat entails way too many calculations and is fraught with chances to make errors.
Notice in the inside of your flanges that the angles aren't even flat.

I know the desired finished dimensions (or at least you do), so I would model the finished part and let Inventor caculate the flat (including bend allowances).

 

[cjjatpuresilica]

Dear rollupswx,

I can only assume my system is not set up correctly for the direct opposite occurs. All the default settings produce lines on my Apple Cinema screen 1.0 to 1.5mm thick; hence my desire to manually alter them.

I must also be somewhat thick as well as lacking in geometric observation for I can find nowhere in the tutorial link you kindly provided how to constrain to a plane, axis or centre point.

I am as previously stated most grateful for your help.

cjj

 

[cjjatpuresilica]

Dear rollupswx,

The edges you refer to should not be flat for they meet at a compound angle. Nothing in the model is at 90 degrees.

Thank you.

cjj

 

[cjjatpuresilica]

Dear rollupswx,

I have looked at your kindly modified version of my file and the problem I have is that I must have the flanges right into the corners. If Inventor cannot auto mitre the flanges it would seem my only option is to form the flanges by sweeping but I still run into problems in the corners. I would have to mitre the first flange before sweeping the next etc.

I simply do not understand why Inventor is falling over with the auto corner mitering?

Thank you once again.

Christopher

 

[cjjatpuresilica]

Dear rollupswx,

I apologise for my earlier message. I had failed to see the Corner Seam you had added.

I will go away and look at this feature in more detail.

Thank you so much.

cjj

 

[cjjatpuresilica]

Dear rollupswx,

Your modified version of my file appears to do exactly what I want - thank you so much.

I recognise it must be really basic information but how did you constrain the sketch centre point to the Origin Center Point. The Origin Center Point does not appear to accept any form of association!

Thank you.

cjj

 

[rollupswx]

I recognise it must be really basic information but how did you constrain the sketch centre point to the Origin Center Point. The Origin Center Point does not appear to accept any form of association!

You must not have read that document I posted earlier.
If you have Inventor set up correctly the Origin CenterPoint will automatically be projected to each new sketch. (it you have by chance deleted the autoprojection at some point you can simply Project Geometry and click the Center Point into the sketch. Now you can add a coincident constraint.) Once you get the hang of Inventor you will see that you can set it up to do a lot of automatic work for you.

Here is how I might model this part (there are other ways). One advantage to modeling in the finished size state is that you can simply edit dimensions to get desired finsished size without any calculations. I didn't know whether your angle or height was the controlling dimension - so I assumed height. This could easily be changed.

I assume from an earlier statement you made that there might be more to this part. Continue adding features and post back to see if there might be other ways.

Of course, becuase my model was done in EDU version - delete it after you have reproduced.

BTW: If you want to tighten up the miter you could do something like MiterGap/2 or whatever. Keep in mind the manufacturing tolerances.

 

[cjjatpuresilica]

Dear rollupswx,

Thank you for all of the information in your last post.

I will look at your part file now and revert tomorrow if that is OK?

Thank you once again.

Christopher

 

[rollupswx]

When you take a look at it the obvious question is, "Why not do as a single Lofted Flange - I tried that and it works, but after mitering the flanges it left a bend anomaly that should have been trimmed away.

Therefore I ended up having to do just a bit more work than intended - adding construction fillets to the profile sketches, 3 lofts instead of 1 and 2 bends that otherwise would have been automatic.

For most parts I could have greatly simplified the Contoured Flanges into one feature with automitering, but the angles on this one presented problems.

But I think you will agree it is easy to set up (no angle calculations) and maybe more important - easy to edit.

I try to create most work in such a way that the sketches are independent of the features. You should be able to describe most of the part from only simple sketches similar to traditional 2d orthographic projection views.