Trying to understand the structure

[bosskoss]

Hello, 

I am trying to create a simple laptop stand.

Very simple rectangular frame made out of 4 pieces of wood and two wooden legs connected with lateral piece, so they form a U shape. The legs can rotate around a bolt that is connecting them to the frame in their upper part. Think of the letter lambda.

What I am trying to understand is the component - body structure. Do i have two components, one for the frame and one for the legs? Or does every piece of wood get to be a component?

Thank you

[etfrench · Accepted solution]

Yes. You don't need the "or" in your question 😀

Joints can only be made between components.  You can have many levels of components and subcomponents.  Subcomponents are components in their own right. 

See Rule#1.

[bosskoss]

Hello etfrench, thank you for your advice.

Assuming I do not want them to move separately, infact if they could stay somehow "bound" together, as a real frame with screws would, so that I can move them around in unison, should the separate parts of the frame component be subcomponents, or just bodies within the frame component? 

How would I bind the parts (whether bodies or subcomponents, whichever is more appropriate) of the frame component together?

[etfrench]

Rigid groups or Rigid joints are used to keep multiple parts aligned.  I prefer to have only a single body in a component or subcomponent.  A top level parent component should not have a body if it also contains subcomponents.

[bosskoss]

Alright, I seem to be getting the hang of this.

So Frame component will have 0 bodies, 4 subcomponents (one for each side) in rigid group, because I've noticed, that with rigid joint you can actually move the components separately.

And the leg component 0 bodies, 3 subcomponents (one for each leg + the lateral piece) again in rigid group.

Thank you.

I suppose I will have a follow-up question regarding how can I actually join the leg and the frame to rotate as I need them to.

[bosskoss]

Alright, so I came up with the design, two main components, frame and legs, each with subcomponents.Rigid groups for frame and legs separately, one join for movement of the legs.

Could you please take a look at it and point out some obvious flaws or perhaps what could be improved? 

I am attaching the f3d file

[laughingcreek]

I usually approach these types of designs with a top down approach.  skeleton sketches on origin planes, components extruded from those.  I avoid using any move commands, position captures, or align commands.  These wreak havoc on parametric designs.

example attached.  Note this if fully parametric by editing any of the sketch dimensions that don't have a fx in front of them .  You don't have to go digging into any of the features (extrude etc) to change things.  A year from now when you want to change a few things you'll thank yourself for setting it up this way.

You also have components that are identical to each other, but are named different.  These can (should?) be 2 instances of a single component instead. (talking about frame-vertical-left / frame-vertical-right and stand-leg-right/stand-leg-left)

Even if you prefer your approach, it is generally better to put the parts together with joints without using move, align, or position capture.  stack all your joints up at the end.

[bosskoss]

Thank you for the model, it helped me to understand so many new things! This is cool!

I can see how that makes the job of changing things later so much easier by simply making sketches for each of the planes. I also learned how you used the R-pattern function, this is going to save some time.

There are a few things that I do not understand though.

What is a parametrical sketch and how do I make it work like this?

Would this approach work for more complicated models? What if I wanted to have another set of holes along the centerline of the legs, for example for some stopper to fix the stand in certain position? But those holes would not go through the vertical frame.

And if I wanted to include Bolts and nuts for the hinge joint and wood screws for the other parts that should be fastened together? Like through the countersink holes? 

[g-andresen]

Hi,

---

@bosskoss wrote:

What is a parametrical sketch and how do I make it work like this?

user parameter

Would this approach work for more complicated models? 

YES

And if I wanted to include Bolts and nuts for the hinge joint and wood screws for the other parts that should be fastened together? Like through the countersink holes? 

JOINTS are your friends!

---

günther

[bosskoss]

Hello,

Thanks! 

So apparently I will define parameters, and then I can use them in the sketch, which then match the dimension and put fx in front of it.

Is to possible to change the defined parameters and would that change immediately affect the sketches and the components? Im thinking that I can define the dimensions of the material I would be using, and in case I would like to use thicker one, I could just edit the defined parameters.

[g-andresen]

Hi,

---

@bosskoss wrote:

Hello,

Thanks! 

So apparently I will define parameters, and then I can use them in the sketch*, which then match the dimension and put fx in front of it**.

* not only sketches > "nearly" all available features 

** is done automatically!

Is to possible to change the defined parameters and would that change immediately affect the sketches and the components?

YES

Im thinking that I can define the dimensions of the material I would be using, and in case I would like to use thicker one, I could just edit the defined parameters*.

---

günther

[bosskoss]

Alright, that is super effective, and I will definitely start using it.

How do I however make my sketches centered at the origin like in laughingcreek's model? Is that possible, or is that done manually?

[laughingcreek]

Based on your last few questions, I think going through the tutorials on sketching would be a valuable use of your time.  Sketching in fusion is different than in other programs, and is a foundational skill needed to pull off good designs. 

[bosskoss]

I've actually figured it out, observing your sketch, I just drew diagonal of the frame and attached it to origin via the centerline constraint.

Now following your example, I extruded top from the front view, but how do I create the hole in it from the top view, using the sketch that is bound to origin?

I am attaching the model.

[davebYYPCU]

By following Alex's file, he has used an advanced extrude technique, to make that hole.  I am not sure why he has done that at this early stage, will let him explain, 

To make it easy, select the two circles in the origin sketch, Extrude them up right through the body, and it will convert to cut in the process

You will have fix sketch 2 before much longer.  Yellow icons should be fixed when they appear, due to the fact that whatever you "just did" is the cause and you should not do "that"

For now, Right click on the yellow icon, select Manage Lost Projections,

1.  Left Click to highlight  

2 Select ReLink

3. OK.

Might help....

[bosskoss]

Hello, thank you for the tip.

I am not exactly sure what caused it, probably while I was changing some stuff in the sketch, anyway the relink wouldnt fix it, so I just deleted the geometry, it was a leftover line from previous version of the sketch, I had to redimension a few things and fix the sketch on origin again, but after that it was solved.

I actually fiddles a bit with the extrude, and since it is countersink hole, I did two extrudes, both starting from "object" which was the top face of the top frame and for the wider one, i simply extruded by -5 mm and for the 3mm hole I extruded in both directions.

Then I mirrored the hole.

[davebYYPCU]

Counterbore hole, explains it, thanks.