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Help with Parametrics gone awry

6 REPLIES 6
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Message 1 of 7
benjaminfelber
178 Views, 6 Replies

Help with Parametrics gone awry

Hello, 

I use Fusion360 for furniture design so generally things stay fairly simple. I rely heavily on the Paramatrics and never have issues.

 

I recently decided to scrap a complex project that had gotten too messy and start over with a different method in which I created an origin body, which has the outer dimensions of my furniture, and construct mid planes in every axis based on the parametric values of the origin body. I sketched directly onto this origin body and extruded new bodies as needed, almost always symmetrically from the applicable midplane using my parametric values, and had the basic structure of the furniture done very quickly.

 

I tested the project by changing the basic metric which is referenced by many of my parametric values by 1mm , and was surprised to find that while the outer dimensions changed accordingling, the separate bodies where joined or cut and no longer recognisable.

 

I'm wondering what I did wrong. 

 

 

FYI : I didn't actually start a new file. I deleted everything in the original and kept the parameters. 

 

6 REPLIES 6
Message 2 of 7
g-andresen
in reply to: benjaminfelber

Hi,

This cannot be answered without an insight into the design.

 

Please share the file.

File > export > save as f3d on local drive  > attach to post

 

günther

Message 3 of 7
benjaminfelber
in reply to: g-andresen

The base dimension in question would be the Parameter Dielen_breite with 60mm changed to 59mm.

Message 4 of 7
davebYYPCU
in reply to: benjaminfelber

Wondering what I did wrong?

 

Nothing wrong, just that some things are better.

Origin is not making use of symmetry, but you used all sorts of symmetry with midplanes. 

Use the Origin for those 1st 3 midplanes.

 

Avoid Box Command if you are going to use a sketch of it later.

Avoid mirror in sketches.

Avoid Mirror in modelling, when Circular pattern will do it.  Patterns will count duplicates, Mirror will not.

Avoid blue sketch articles, when using Parameter changes.  (Trouble with capital T)

 

It's very hard to find where this parameter (Dielen_breite) is used, Looks like a part of formula.

 

Your timeline is very hard to understand.

I have checked as far as the first Combine icon, (why) in some extrudes up to there, you have stopped using parameters, and just new data dimensions.

The extrude errors are mostly in this Deckel(Mirror) component.

 

Changing Dielen_breite to anything else is breaking the extrudes without parameter data and or the blue sketch articles., as best I can tell. (Not english labels)

 

Later in the timeline you have Move and Press Pull icons, both of these tools are not going to help, either.

 

Might help....

Message 5 of 7
benjaminfelber
in reply to: davebYYPCU

Thanks for the feedback.

Let me paraphrase to make sure I'm getting everything.

 

1. Mirroring in sketch is very bad; constraints don't get mirrored with.

2. Mirroring, press/pull and move/copy in solid is bad; instead use pattern. why is this?

3. Blue lines are very bad; no constraints. 

 

I have checked as far as the first Combine icon, (why) in some extrudes up to there, you have stopped using parameters, and just new data dimensions.

 

Do you mean the Seite extrudes from profile plane to object? Would it be better to sketch with a parameter?

Message 6 of 7
davebYYPCU
in reply to: benjaminfelber

Sort of, generally you are working too hard, and

then losing the process as you work along the timeline.

 

Depending how far you are parameterizing, 

The extrudes that broke, were in the mirror top frame sheeting, I didn't quite pin it down - now I am thinking it is the blue sketch items on top rear.  These extrudes were just dimensions, but earlier you had parameters driving the work.  (Bottom frame did not break)

 

So a normal cabinet model would have 4 long rails and 4 short rails of the same material, so I would do one part, joint one corner and use patterns to get to the 4 each set.  Mirrors will give 2 left and 2 right, but they are the same size, so a BOM would need to see 4 count.

 

It is also more normal for one component / one body, and duplicate the components with pattern.  You have duplicate bodies in one component, but Joints don't work with bodies.

 

So your statements 

1. Mirroring in sketch is very bad; avoided constraints don't get mirrored.

Fusion sketch does not like Symmetry constraint.  Draw full rectangle.

 

2. Mirroring, press/pull and move/copy in solid is bad avoided; instead use pattern. why is this?  See above, and 

Depends on the job, mirror half to make one body and mirror 1/4 twice to make one body is fine, 

Press Pull is not using the sketch to control the body / Component, you will lose control.

Move in sketch is good, Move in the timeline causes trouble, 

Pattern components saves time, make one, copy many.

Components can be Jointed.

 

3. Blue lines are very bad; no constraints.  Correct.  Make all black.

 

Extrude Tool like you have it is OK.  But the sketch was blue.

Try Rule #1, one component for each part

For your front door, do one and Mirror it, because it has to be one left and one right, this is OK when needed.

 

Might help....

Message 7 of 7
benjaminfelber
in reply to: davebYYPCU

Dude, this is insane. You just opened up a whole new world of fusion for me. I'm going to be studying this for generations to come.

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