Problem with resizing

[chadbingham52]

I guess, the real problem is not resizing, but with bad constraints, I think? I am designing a hutch and it consists of three components, base, middle, and top. I realized the middle component was too tall. I tried to resize it and I didn't get the results I was expecting. After I resize it, I am given this healthy list of errors and warnings. I am very new to this, so I couldn't decipher well enough to fix my problem. 

These were the errors:

Warning: Extrude4 1 Reference Failures
The profile reference is lost and this feature is using cached geometry.
Edit this feature and select new profile references.

Error: Split1

Compute Failed

Warning: Shell1 1 Reference Failures
The face reference is lost and this feature is using cached geometry.
Edit this feature and select new face references.

Warning: Panel1 1 Reference Failures
The sketch plane is lost, Cache is used. Please redefine the sketch to select other plane!

Warning: Panel2

1 Reference Failures
The sketch plane is lost, Cache is used. Please redefine the sketch to select other plane!

Warning: Extrude6 1 Reference Failures
The profile reference is lost and this feature is using cached geometry.
Edit this feature and select new profile references.

[Drewpan]

Hi,

Exactly how did you "resize" your model? It is difficult to tell from the timeline. Most of those errors are because

things don't line up or are different measurements. I can clear some of them but I am not exactly sure what you

are trying to do.

The first is simply that you told it to extrude something but it lost the profile. When I select the sketch profile it

creates a box and clears.

The split body fails because the plane you created doesn't cut anything.

If you make a plane using the top of the shape and offset it the same distance below that surface and use this plane

to cut then it works.

Your resize has caused the shell to fail because it is shelling what isn't there, if you change it to a smaller value it

works.

The next failure is caused because the sketch plane has been lost and just needs to be redefined.

And then you try to cut thin air.

What exactly are you trying to cut? The yellow marked line is the cutting surface but it does not pass through any

bodies to cut. The blue area is a sketch hanging in mid air that seems to serve no purpose. The red area seems to

be a backing of the unit but because of the resize now hangs out in mid air.

The next warning is simply redefining the sketch plane.

From here it goes pear shaped as the cut of the non-existant body is critical geometry for further operations and

since I can't work out what it is there is no point going on.

My suggestion is go back to the last version that actually worked. This one is version 9 so if version 8 worked

BEFORE you tried to resize it then start again from this version.

One other thing I noticed is that you seem to have redrawn the sketch of each part when you could have used the

original and simply offset the extrusion from where you wanted.

A tip to follow - warnings in the timeline should be fixed AS SOON AS THEY OCCUR. If you break something then go

back and try again a different way or correct your mistake.

I would also STRONGLY advise you to read the documentation and do the embedded tutorials and self paced

learning. The time spent doing this is NEVER wasted. I frequently go to the docs to check stuff when I am not sure.

When I don't I usually get bitten answering posts on the forum. Nobody is perfect.

Cheers

Andrew

[chadbingham52]

Thank you for your answer, it has been insightful. I resized by changing a value in my Parameters. After I did that, a series of things were broken. What I struggle to understand is what? I see a profile went missing. What did I do, or didn't do, rather, to cause this? Can I fix it, or do I need to go back and do it again?

[davebYYPCU]

What did I do, or didn't do, rather, to cause this?

Most likely, you are not tying reference articles into the change of parameter requirements.

Dependent on design intent, when you start a second sketch you harvest existing articles into the sketch while it is empty, Project > Project and Project > Intersect, should be step one in all subsequent sketches.  Saves time and stops parameter changing errors.

Can I fix it, or do I need to go back and do it again?

if changing a parameter breaks the timeline and or the model, then it’s start over from the broken part, test the changes as you build it.

Might help….