how to re-use/copy the same part but with different lengths

[Anonymous]

I expect this questions has been asked before, but I cant seem to to find it the appropriate answer. I am new to fusion 360 with only a few designs. I am currently designing my own cheap 3d printer using extruded aluminum square profile. I created a sketch of aluminium profile and set user parameters for depth, width, thickness and length with the length equivalent to the extruded length. What I want to do now is create a new part but with same parameters but with a different length. I can copy the part and change the new part by re-extruding the length  but that seems not to be particularly smart way of doing this. I did try a addin from called fusionsheeter as I thought it particular interesting option, but unfortunately google blocked the app and I was unable to get that resolved (that;s another story off topic). Can you provide a simple explanation of how do I go about creating a part (or component) that I can reuse but change its length. Appreciate your assistance.

PS. What I did find on the forums was reference to components but I couldnt see how this would help as copying a component is just like making  a clone and changes on one component effect all others, but that may be my poor understanding. You can create a new component but I am not clear if this copies the user parameters but I haven't tried that yet.

[davebYYPCU]

Not enough info to help here, but 

Lets say you are doing Core XY, a cube with 12 parts to make the basic frame.

That would be at least two parts being duplicated, but will go with 3 (LWH)

Make one and copy Paste New the other 2 making changes to the part 2 and 3. 

So profile sketch.

New Component.  (L) Make the first part and Copy 

Paste New 2 more copies (W) and (H).  Edit these part lengths.

Mirror or Pattern these masters

or Copy those parts as Copy Paste - 4 of each to keep relativity. 

(3 basic Components with 4 of each = 12 parts)

Might help....

[jhackney1972]

If you make the Length a parameter, when you Copy and Paste New, the parameter table becomes unmanageable because the two, more or less, static width and height are replicated.  If you edit each Paste New component with a unique length parameter, it is a lot more manageable.  You will always have the ability to change the width and height of all in one shot, if needed.

[arwalker324]

Fusion 360 has the concept of derived parts (designs), but they're no help here because it doesn't work within a design, between components or bodies and as the whole concept of Fusion 360 is to have an entire product/assembly in one file (unlike Solidworks that have a file for each part - I forget what AutoDesk call this approach), it seems a bit strange. What is desperately needed is an equivalent to SolidWork's "Configurations".

What would be nice is the ability to have a halfway house between paste and paste new, where there's an option to retain the link to the source profile sketch(es).

If you have a common complex profile that you will change and have components with differing lengths but the same profile, the way I often do it is to create the profile' sketch outside of the component, create the component and use the profile sketch to create the component's body.

Given the above tree for a french door, at the moment, I have three frame sections and the threshold:

(1) is the top level

(2) is the entire frame. Threshold and 3x frame sections.

(3) is the profile sketch ("Frame profile"). Note, it is outside, or above the frame sections.

(4), (5) & (6) are extrusions using the profile sketch ("Frame profile").

If I make a change to the profile sketch ("Frame profile"), all 3 frame sections are updated.

I get that this doesn't work for every design and depending on how unique the "derived" component is, it might not be any help, but that's the best I can come up with at this moment in time.

HTH.

[jeff_strater]

Configurations in Fusion is currently in development.  We hope to release it later this year.  A preview will be available through the Fusion 360 Insider program fairly soon, I believe.

[arwalker324]

Hi Jeff,

Yeah, it looks really good. I can't wait. I signed up to take it for a spin, but I haven't been selected (yet).

I thought "Insiders" were under NDA and not allowed to mention things in the insiders track in public forums.

T, A.