Insert, Unlink, Position, and Feature Edit

[PrecisionDesign]

I have realized that the biggest downfall of F360 for my applications will be the lack of being able to edit features after positioning unlinked components. I use mulitple stand off components in our equipment designs which consist of identical components that only vary in length. I have created a base file that I can insert into my design, unlink, and position. My intent is to then use this position to drive the length of each stand off to a common faceplate...but because of the timeline order when I edit the extrusion feature that drives the length it defaults back to its position that the component was created in. Not real sure how to get around this, seeing that the captired position can not be moved before the feature that the component is generated from.

The way I have got around this is by creating a minimal base length and then doing a second extrude in position, but doing this makes my OCD flare up slightly. I also have to go back and add the mounting holes for each stand off seperately instead of having a base compnent that would just need a single length edit, this adds time and frustration.

THOUGHTS??,

Brandon.

[Beyondforce]

Hey @PrecisionDesign,

Will you please create a screencast, so we can see what and how exactly you are doing it!

Cheers / Ben
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[davebYYPCU]

Sounds like you only need a Press Pull on the face of the / many post/s, to align to the faceplate, which will not require you to go back in time. 

will depend on the structure of the file / assembly though.

May not be that simple, without additional information...

[PrecisionDesign]

Sorry about the audio, I think it is time for a laptop upgrade.

[Beyondforce]

Hey @PrecisionDesign,

1. When importing a component, use the move command to position the component where you want it to be and. Very easy to-do. Let me know if you need help with that. The position should be captured as well, otherwise, it will jump back to the original position.

2. If you want to edit a linked component, then you must open it first, save it and then refresh the assembly file in order to see the changes.

I hope this helps.

Cheers / Ben.

[PrecisionDesign]

Ben,

I am able to position the Tab Risers fine.  This is not the problem.

1) I UNLINK each tab riser because each one will be of a different length derived from the distance from the face plate in the assembly file.  Therefore I don't see the benefit of having them linked to a base file that would need to change depending on the length required.

2) If I was to keep the active Link and edit the length of each tab riser in a base file I do not have the option of driving the length of the riser by the face plate because it is not part of the base tab riser file.

[Beyondforce]

It is very difficult to see exactly what you are doing, but you should work on your symmetry! Your assembly is waaaay of the origin center and I'm not sure how you did that. I'll fix that first if I were you.

It will be much easier to help you, if you could share the model. Which it wouldn't be easy to do right now, since Fusion's cloud is down 😞

[PrecisionDesign]

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@Beyondforce wrote:
It is very difficult to see exactly what you are doing, but you should work on your symmetry! Your assembly is waaaay of the origin center and I'm not sure how you did that. I'll fix that first if I were you.

It will be much easier to help you, if you could share the model. Which it wouldn't be easy to do right now, since Fusion's cloud is down 😞

---

The reason for the design position is because the requirements of the equipment is to be designed in "Car Position" which is standard pracitice and should not be an issue as long as you use proper construction refreneces and geometry.

Brandon

[Beyondforce]

If you don't mind attaching the file, that would be great.

[davebYYPCU]

Gooday Brandon, 

After the video, I would change tack a little, and make your short component too long, with long threaded holes, 

When assembled in position, use a top down extrude cut, aligned with the front of the mounting bracket, and cut all 12 components at once.

Some pic to show what I mean, before and after, Might help...

[PrecisionDesign]

I appreciate the assessment from a different vantage point. This solution removes the extruded step required for each component, but would still require the mounting holes to be added seperately to maintain a consistent depth. I appreciate the input and will incorporate this option at my next opportunity.

Brandon

[davebYYPCU]

Do the holes exist in the mounting bracket, or are they developed from the cut component/s?

I am thinking, the component does not need the holes only the set out sketch, 

After trimming the length, create a sketch on the bracket face, project the hole positions, then drill / tap and countersink as required, from the one sketch,

Might help, realise it is design dependent.

[jeff_strater]

Sorry, late to this thread.  If I understand correctly, what you want, @PrecisionDesign, is something like this:

• a component that defines the "base shape" of a component
• the ability to instance that component, but have different variations of its shape
• still maintain a relationship to that "base shape" so that edits will update the top level instances

If so, there are two usual approaches to this in a CAD system:

1. component "configurations" or table-driven components.  In this type of a system, you can describe all the variations of a component via a table of values (dimension values, pattern counts, etc), and be able to choose a row in this table at instance time.
2. "assembly features".  In this approach, you can instance the same component, but make assembly-specific edits to instances of that component.  Sometimes, those are limited to material removal, but I don't think there is a real reason for this.

Unfortunately, Fusion does not have either of those at this time...  

There are some kludgy ways to work around this.  One involves copying the body from a referenced component, turning it into a different local component, and then modifying the copies.  It's pretty limited, but you can do some basic things with this.  It might not work in your case, but if you are interested, I can throw together a quick screencast.

Jeff

[PrecisionDesign]

I think I have figured out the proper workflow to be able to move components and edit features in position after breaking a link without creating errors.  I would use this when I have multiple identical components that just vary in length driven by a common plane (i.e. Mounting Plate)

The key to this is to create an initial reference plane to hold the first sketch, which can be moved to other locations in an assembly when the inserted components link has been broken.

My issue was that I wanted to change the length of a component in an assembly position but because the length was created in my first feature it would default back to the plane that sketch was created on (X,Y,Z Plane Origin).  I was not able to drive the length "by object" to keep each length parametric to the face of a mounting plate.  By creating a reference plane to hold our initial sketch, which can be edited and moved around after a component has been inserted and unlinked, it allows us to reference a new position for that component by changing the selected geometry to create the reference plane holding the sketch..

NOTE:  Care has to be taken in the type of reference plane to use for this initial sketch creation, it should match available geometry types for plane creation at the positions to be moved to in your target assembly.

Brandon