Changing a parameter breaks a well-constrained sketch

[popvotocek]

Hi! I have a case for an electronics project I am making. I attached the f3d file below. The dimensions of the case and the angle of the front panel are defined by user parameters.

The front panel angle is 25 degrees

 

There is a sketch on the inside of the front panel ("frontPanelSupport") that has screw holes along with a lot of rectangles and offset lines. I would say that it is pretty well constrained. There are coincident constraints that keep the sketch geometry aligned with the wall of the case (it is projected on the front panel sketch as it comes from the "case" body)

Now, the problem occurs when I change some parameter of the case. For example, I changed the frontAngle from 25 to 20 degrees.

After this change the sketch completely misaligns even though it is constrained.

The body breaks too, of course.

 

What could be the problem? How could a sketch misalign like that?

Thanks

[TheCADWhisperer]

@popvotocek 

I haven't found the issue yet, but I have already found several things that I would do differently:

1. I would make use of obvious symmetry about the Origin...

2. I would pattern Features rather than duplicating sketch dimensions and symmetry (mirror) constraints...

3. I would most definitely do this fanGrillTexture sketch as a single fully defined hex and pattern Feature rather than sketch.

Now let me keep digging... 

[TheCADWhisperer]

...continuing on...

I grouped duplicate dimensions together.

I would significantly simplify this sketch.

Each dimension is requires only once and pattern features rather than repeating sketch elements...

[TheCADWhisperer · Accepted solution]

@popvotocek 

What happens if you Delete this Tangent Constraint (and perhaps the 180° dimension)?

[popvotocek]

Thanks a ton for your replies!😀 That was it. This tangency constraint was an error and it was breaking the whole sketch. I replaced it with a perpandicular constraint.

[popvotocek]

Yeah, that 180 degree angle was a weird constraint too. I don't know why I thought it was a good idea to put it there:D

It is true that this sketch is really overcomplicated. It just shows that I am not very experienced yet. 

I don't fully understand what you mean by the fact that each dimension is only required once though. They all serve their purpose in different areas. Could you please elaborate on how you would go about simplifying that?

I suppose by patterning features rather than sketch elements you mean just the mirrored parts of the sketch, because other elements are different right?

Thanks!

[TheCADWhisperer]

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@popvotocek wrote:

I suppose by patterning features rather than sketch elements you mean just the mirrored parts of the sketch, 

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@popvotocek 

No.

Keep sketches simple...

In order of preference from least computationally expensive to most computationally expensive...
Pattern Components 

Pattern Bodies

Pattern Features

and last if not a better way

Pattern sketch elements.

See Attached file.

[popvotocek]

Wow, thank you for that tutorial. That really helped me a lot and I learnt new methods from the project file. 

Thanks and have a nice day!