Critique of My Skeleton (CATIA)

3D Design Volume Model
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Hi all

Since practice makes perfect, I tried to make my first skeleton with CATIA. And I'd love to have your feedback on that.

Is it a real skeleton or I still didn't understand what it was?

Have I forgotten any tips or tricks to make my life easier? 

Is it accurate enough (or even too little or not enough)?

In short, all advice will be welcome.

CLARIFICATION: I want to make a skeleton for assembly (the one I'm presenting to you) and that I'm going to try later (with the other people in my group) to make skeletons for the parts. 

Thank you in advance for your answers.

Ju"


squelette.png
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Attached is the part file for people with CATIA.

Note that this skeleton was made using the V5R18 version.


skeleton.catpart
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Hello

In principle, there are no problems, it's a skeleton. In any case, there is no absolute rule. It is to be adapted to your needs.

Some people sometimes prefer to place markers at strategic points. It saves time by making the landmarks of the skeleton coincide with that of the piece to be placed.

Just a remark, I see that you're in hybrid design (the volume and the wireframe are mixed and the part body icon is yellow). It is often recommended (or even imposed in some companies) not to use this mode. You have to change it in the options or when the "new room" window appears.

It's a bit similar to your idea of making a skeleton for your parts. No need for a separate file in this case. By disabling the hybrid design, the point, wireframe or surface elements will be placed in a "geometric set" (you can create as many as you want in the same catpart file to sort => insertion => geometric set) and the volumes in a part body (same as for geometric sets, you can create several but be careful, In this case, the bodies are not merged with each other. It can be useful when you want to make welded assemblies for example).


option_conception_hybride.png
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Hello Chamade,

Thank you for the answer. Oh yes, I hadn't thought about the idea of landmarks, it's not too bad.

Oh I don't know that at all. (It's typically this type of little detail that I'd like to know, because they can ruin a job.) You mean that the little gear is yellow instead of green, right? 

If I understand correctly, geometric sets are only used to include 2D elements (point, line, etc...).

While the parts will allow you to create volumes (as you can do when you create a room on your own).

Another point if I create multiple part bodies, the bodies are not going to be merged. This means that Catia understands that I have a body A, a body B, a body C, (etc) and which are all different? So this ties in well with the idea of an assembly with a multitude of different parts, doesn't it? 

 

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You may be missing ref plans to come and rely on it 

but I think you can add them as you wish via the evolution of your design

@+;-))

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@julien_2, yes that's right, you got it right.

For the question of the parts bodies, we can see it as a kind of assembly but you will only have a catpart file. So it is generally only used for elements that are ultimately unremovable from each other and considered as a single block (e.g. mechanically welded structure).

To make a fuselage for example, it is cleaner to make different parts for the frames, the skins, ... even if the whole thing is not specially made to be dismantled.

In fact, you can see this depending on how you plan to make your plans. If you only make one plane for several elements, make bodies in the same part. If you want to make separate shots, make an assembly. (even if it's never too late to change your mind)

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Hello.

I agree with Chamade about the hybrid mode, to put it simply.

If the mode is active, you cannot reorder the surface and construction elements before the parent. (e.g. I create a plane // by a point I cannot reorder the plane in the tree before the point.)

These same elements can be included in part bodies with the same rule.

If the mode is idle, these elements cannot be included directly in a body and do not meet the parent organization rules.

It is important to know that it is extremely difficult to transform a hybrid model into a non-hybrid.

Skeleton.

For an assembly skeleton, I know two types.

ASS by compulsion.

The skeleton represents the position of the components in the assembly.

Each component is designed to be stored on the origin (e.g. for a screw, the axis of the screw on Z, the point of origin (X-0. Y-0; Z-0) is coincident with  the bearing surface of the screw.

This type of assembly is very useful when there are a large number of parts that are standard components or machined library parts that can be used in other projects.

ASS In position.

The skeleton controls the position of the geometry of the components.

The origin of the assembly is common to most parts or sub-assemblies.

(this is where it is convenient to create markers) the published elements (marker or other) are copied and pasted with a link in their respective parts or subsets.

The only assembly constraint used for each part and sub-assembly is "fixity".

In each piece we design not on the common marker but on the one pasted with an "external ref" link.

From assembly, changing a position moves the geometry inside the part or S/E.

This type of assembly is widely used for injection molds (for example).

Remarks after opening your file.

There is an Inactivated formula (we very frequently have elements in a skeleton that we activate or inactive) so we have to be very careful, not to leave this type of elements if they are not necessary.

A few unnamed points.

You have to keep in mind that this will very quickly become a gas plant so use all the features of CATIA to simplify the skeleton (e.g. using the "surface workshop" symmetries it saves formulas etc if several lines, curve are intended for the same part the "assembly" surface function is very useful.)

 

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