Parametric "move"

[bkgoodman]

I've created a box wall which is "width" wide ("width" being a user-parameter) - using "width" to define the length of the composite lines within the sketch from which I extrude the "wall".

I move this wall into the correct position by "moving" it, and specifying "width" as the parameter to have it move by - and all is good, wall is now in correct position.

However, when I change the "width" user-parameter, though the sketch and extruded wall change their sizes accordingly, the "move" operation just stays where it was.

Also, when I go to "edit feature" in the timeline on the "move" operation, all the movement parameters are zeroed. Thus, it appears the move operation has little "memory" of what it did - and thus does not "reply" on the timeline from the user-parameters which were given at the time - as it does with a sketch.

So,

1. Is it supposed to work as I describe?

2. What am I doing wrong?

3. If it's not supposed to work like this - how can I get it to work so my objet "moves" into the correct place, when the user-parameter which should define it's relative position changes?

Thanks!

-BKG

[fritter63 · Accepted solution]

Try specifying it as a joint rather than moving the object?

[jeff_strater]

You are not doing anything wrong.  This is a limitation of the current Move command.  We are working on a solution to this to allow you more effectively edit Moves.

In the meantime, as @fritter63 says:  If you are moving a component, try using a joint.  That has the added advantage of being associative.  Another choice is to use the Align command that will allow you to align bodies or component by aligning geometry (face/face, etc).

Jeff

[EDukeCNC]

What Kind of joint would you use, I cant seem to define the location very well

---

[g-andresen]

Hi,

1. rigid  joints

How to:

1. create components > bodies don´t work

2. create joint / rigid > select 1. plane > hold ctrl(fix direction) >select point > same for second component

3. compnent are jointed

günther

[Allitnil]

I also came across this limitation today.

For anyone interested, or for future reference, this was my scenario ...

• Insert two prebuilt components, (push) buttons, for instance.
• The buttons are reusable components (linked) and could be updated in the future. The buttons are different types, so they have different dimensions. Each button is designed to move as you'd expect (the shaft has a sliding joint).
• The buttons must be positioned parameterically, relative to the TOPS of each button.
• The base of the buttons must sit in the holes of a support structure (e.g. a casing). The support structure should adapt its shape to the buttons' positions and dimensions. The support structure is made with additive or formative manufacturing (e.g. plastic).

It seems simple enough until you've many buttons of different dimensions, each sitting on different planes/angles. So to "solve" this scenario I used sketches/axes/planes to define points (in 3D space) for the positions of each button, parametrically. I then attached a joint origin onto each point. I jointed the tops of each button onto the joint origins.  Finally, I used lofting/combine to create the support structure around the button bases.

This method is really powerful for creating an adaptive support structure around the buttons.  However, it feels like an abuse of joints because the tops of the buttons are anchored to the parametric sketch/points, rather than the button bases anchored to the support structure.  So, if you want to "use" the buttons in Fusion (e.g. simulate movement), they don't work as you'd hope.

Can anyone think of a better approach please?  Have I missed something?  I also tried using align, ground and as-built in various combinations, but no luck.

It feels like a chicken/egg problem, that (as I think Jeff hinted) would benefit from parametric positioning in addition to joints.

Thanks!

[CargoFlyer777]

Use the Translate option instead of free move in the move dialog box - it may take more than one move depending on what you are doing, but it does work parametrically 😁👍

[kennedy.timothy.f]

Found this almost 7 years later.  As CargoFlyer777 indicates this will work if using the Translate option, but does not work with the free move.  This is not obvious from a users' perspective, but glad to see this was implemented.

[laughingcreek]

for bodies and faces, the move options other than the first one are parametric.

for components, by design they are positioned with  either joints, or by building"in place".  that's unlikely to be changing. 

[harvey_j_golonka]

This issue appears to now have been resolved as of yet.

Is that so?

[jrmhughes]

Thank you!!   That's not obvious from the UI but I replaced my free move with a translate and a rotate which are working parametrically 😁.

[crkufreak10]

It seems as though the rotate option in "Move/Copy" does not work parametrically. The thing I'm working on is kind of a tough workaround without that.

EDIT: It works fine with bodies, not with components. Which is fine for my use case.

[laughingcreek]

seems to be working for me (see video).  if you can show a case where it doesn't, I'm sure AD would like to see it.  they are constantly fixing things, but really need an example of something not working in order to really do anything about it.

OTOH-it sounds like you are probably not using a good workflow.  move isn't used in parametric modeling as frequently as in other types of modelers.  in fact, it's pretty rare to need to use it.  if you can post an example of what your trying to do, I'm sure someone here would show you a better, and probably easier, way that doesn't involve the move command.

[jeff_strater]

"EDIT: It works fine with bodies, not with components"

Yes, this is as intended.  No component moves of any kind (rotate, translate, free move, component drage) are "parametric".  Any component move just puts the design into a "capture pending" state.  You can use Capture Position to record it, but it will still not be parametric.  Body move, though, with translate and rotate ARE fully parametric.  I know you know this, just explaining in more detail for others.