Cannot extrude sketch (tried everything I could find on this forum already)

[Anonymous]

Dear Inventor users,

I am currently designing 3D printable infill patterns in Inventor but when I have drawn all the lines, the extruding does not work. I tried 'Close Loop' multiple times but even then I manage to find a certain open loop somewhere. The function does not really work for my model. I only drew half, planning on mirroring the sketch after I can get it to extrude. File is attached. 

Hopefully someone knows the solution to this problem, it has keeping me busy a few days now!

[S_May]

@Anonymous

[Anonymous]

@S_May, What did you do exactly? I cannot find this 'tool' to repair sketches, the tensil file attached is not extrudable (Inventor '19). 

Kind regards

[mdavis22569]

Hi @peterjuice

That looks to be an older add-in program ..

However,I ran the Sketch Doctor on it .... a lot of issues were found:

[Anonymous]

@mdavis22569,

I found the docter and these issues but I literally checked every line to the point I could not zoom in any further. I deleted all the useless lines and deleted those. I still get a lot of issues but I want to get rid of those. Is there a solution for these issues?

Kind regards

[mdavis22569]

I found quite a few point issues too ...

Was this made in AutoCAD or something else and imported / pasted in?

[Anonymous]

Hello,

I made it from scratch in Inventor 2019. The infill pattern is already sized up a 100 times (in the beginning, when it is done I want to scale it down, pattern was not accurate enough to do it without upscaling), I made a pattern for the continuous lines and trimmed those when they were out of the boundaries of the tensile test dimensions. I tried it before on a smaller one, there I got it working (the dimensions changed so I had to make a new one and now I can't get it to work). That file is also attached. (this file is made manually in total since the pattern function is not accurate enough, I really don't want to do that for the bigger one since it cost me a lot of time).

I hope this information clearifies some questions for you.

Kind regards

[mdavis22569]

Wondering if it would be better to make the overall ... and extrude cut the inside ..then pattern that extrusion.

A lot less lines / sketches / patterns

[mdavis22569]

Do this one ... part 1 up and 1 down .... then across. You do the end extrusions.

Then you don't need most of these lines and should be a lot faster for the modeling

[Anonymous]

Sorry I do not understand completely what you mean. Do you suggest cutting out the squares instead of building the framework? I think that is quite hard since some squares are cut at a specific point (the infill pattern has to be identical to the one I 3D printed since I am performing a FEA on the model)

[mdavis22569]

I wouldn't do all of the lines you show ..

It's showing 887 missing constraints. That right there is a huge issue ...   One accidental click wrong / moving of a line etc it could mess up everything else very easily. 

[Anonymous]

What do you mean with not doing all the lines I show? Making a smaller sketch? I have to have the exact same dimensions and amount of squares.

[mdavis22569]

For all of the patterning / removed area you show, I'd cut them out after vs modeling them in the beginning.

[JDMather]

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@Anonymous wrote:

...The infill pattern is already sized up a 100 times (in the beginning, when it is done I want to scale it down, pattern was not accurate enough to do it without upscaling),

... That file is also attached. (this file is made manually in total since the pattern function is not accurate enough, I really don't want to do that for the bigger one since it cost me a lot of time).

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I don't have time to demonstrate how to correctly model the geometry at this time, but your statements do not  make logical sense and your technique is not the best/easiest/robust technique that I would use.

Model 1:1

Pattern Features rather than Sketch elements

or

Grill feature.

You are doing too much work to create simple geometry.

Show all constraints - what do you see?

[JDMather]

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@mdavis22569 wrote:

For all of the patterning / removed area you show, I'd cut them out after vs modeling them in the beginning.

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I would do just exactly the opposite.

I would cut and pattern or grill at the beginning and then trim and add the ends.

(In this case probably Pattern rather than grill.)

Why, because the ends and boundaries of the mesh are different than the rest.

Think of this as trimming a desired area from a larger mesh screen for a window bug screen.
Before the stock screen material is trimmed - it is uniform (up until the boundaries).

[Frederick_Law]

Great idea.

I wonder how to cut infill out but never though to build part around it.

I always want to shell the part then intersect a block of infill so it'll fit inside.

Or intersect infill with solid part then combine with shelled part.

In another word, make a block of infill pattern first.

Cut it down to fit inside part or extrude part to overlap some of the infill.

[Anonymous]

Since the infill lines are 3,5 mm thick in a very specific orientation, the pattern function is not precisely enough. In my first attempt (second file I uploaded), I drew 4 or 5 squares and selected the first or second full line and used the point-to-point distance of those two (which were checked correctly). When I zoomed in very closely, the lines dit not correspond with the fourth and fifth line I had already drawn. The pattern function did not work on such a small scale.

I decided to draw the model a 100 times bigger than it really is and scale it in the end. I am considering to change the orientation of modelling. Instead of making everything diagonal, I thought of making a horizontal plane with these squares. The tensile specimen will then be drawn diagonally and trimed to both sizes. Is that a possible solution? I think it also is like how @Frederick_Law described it.

[Frederick_Law]

[johnsonshiue]

Hi Guys,

This is another profile recognition issue. Indeed, Inventor does not handle this kind of sketch well. Inventor recognizes sketch profiles by sketch constraints. As a result, when there is no constraint between sketch geometry, the given profile would not be recognized. We are working on a solution which will resolve the issues. If you are interested, you can sign up Inventor Beta (https://bit.ly/InventorBeta) to try out the Beta build.

Many thanks!

[JDMather]

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@Anonymous wrote:

... the pattern function is not precisely enough.

... When I zoomed in very closely,.... 

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What?  

When I create the geometry - it is precise out to 15 or 16 decimal places, in other words, exact.

Are you eyeballing pixels on your screen? 

Can you show Measure distance?

I noticed that your work was not created properly and not constrained properly.

Q. If you could create an exact pattern - is that your goal, or do you want a "random" distribution that looks like an exact pattern until observed more closely?