Keeping sketch and component together, or transferring sketch into component

[Anonymous]

I'm working on an assembly with a bunch of different parts. The construction elements of the sketch I used to create this part are referenced off the assembly. I got this far and decided I wanted to rotate and move the object around, to check how it's fitting with the rest of the assembly, but I also wanted to keep it aligned with the sketch it came from so that I could keep using the Extrude, Loft, etc commands from the sketch to add and take away from the geometry. I don't want to have to bring the component back to its original orientation every time I do this. What would have been a better work order? I get now that I broke Rule #1 by not creating the component first and then the sketch, but is there any way I can move the sketch into the component now?

[melvinbrian3d]

i dont think is possible, because those sketches re tied to the main project 😞

[Anonymous]

Another question is whether there's any way in a spot like this to decide to just copy the component into a whole new file along with the sketch.

[sanket223.patil]

I am also stuck to same thing . I also need to move thing along with sketch. Creating components first is better way.

[TrippyLighting]

If the sketch was created by projecting geometry for other sketches or from body edges than you cannot move it into the new component anymore AND maintain the relationship to the original reference geometry anymore.

If you would want to move it, you'd need to break all the links and possibly the reference to the sketch origin if you started the sketch on other geometry. Then you might be able to move it.

[melvinbrian3d]

you can try this...

create a new component, then drag this empty component to the first spot of the Design history, then you can start moving the sketch to this component it will drag any body extruded from this sketch into the new component.

[markusbarnes]

You're correct!  This is the best way to do it.  Return as far back as possible and drag and drop sketches to the newly created component.  I used this to break up a big component into smaller component with their respective features and sketches.  

[taisheng]

Thanks! It really works!

[Drewpan]

Hi,

Yes you did break RULE #1 but many rules are guides that you ignore at your own peril.

As @TrippyLighting says, you can only move things around if it doesn't break the links with other things. You are

much better off planning ahead and not having to move anything, but it does sometimes happen.

In terms of sketches and where they should live and why, it really depends on what you are designing, how complex

it is and, as you mentioned, is it related to other assemblies. I have used both a sketch in the main file and a sketch

with the part.

If the design is relatively simple then it doesn't really matter BUT, as a Designer and/or Engineer it becomes a case

of creating good habits and being consistant. There are arguments and design guidelines for both methods but I

feel doing things the same, correct, way each time is a better habit to have.

I find that I place my sketches in the main part, but if I create assemblies or must match another assembly, that I

place sketches associated with the assembly at the top of the assembly. It is about forward planning as you do not

always know how complicated a part or assembly will get. You also want to plan things so that it is easier to make

changes later if necessary.

A few suggestions to help your workflow.

The screenshot you have shows your part hanging out is space. Is this because you designed it in place or are you

designing it and then using a joint? Both methods are valid under certain circumstances. One thing you should NOT be

doing is MOVING parts around - it clutters up the timeline and causes issues. Either design parts using the Origin and

use a Joint or build them in place. If you are building in place then use Projection off the original part to orient the

sketch. I can see you have projected some points, but I also see a bunch of open points in the sketch that normally

means the sketch is not fully defined. Always fully define your sketch as it is less likely to break something later down

the track.

Why are you using Contact Sets? Contact sets do not work well with Fusion. A Joint with a Motion Link where you have

correctly lined everything up should not cause interference between parts. Use the Interference tool and a cross

section and zoom in close to line things up correctly.

Another thing RULE #1 says is NAME YOUR STUFF. You have a bunch of Components with no names. This is a simple

design but if you said to another Engineer I am having problems with my "Component 1" he will not have a clue what

you are talking about.

Cheers

Andrew

[laughingcreek]

hopefully in the 6 years since nate posted this he's figured it out.

[Drewpan]

Hi,

I hope so too! 😁

I didn't look at the date, just a no solution post at the top of the forum feed.

Cheers

Andrew