How many models are in FreeCAD? (very basic question)

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arcol
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How many models are in FreeCAD? (very basic question)

Post by arcol »

Hi,

I always wondered when I create a model through Part design workbench
(sketch -> pad -> slect a face -> create another sketch -> pocket -> etc, etc), how many models are in FreeCAD?

I mean each step is a new 3D model, and the new step simply hides the previous' step model in 3D view?

If I go to the Edit->duplicate selection, do it create a set of new 3D objects?

Is it advisable to have some independent object in the same freecad document?

I think I miss here the basic concept. I was looking through the freecad document on the wiki, but it did not address this question.

Summary:
- How many independent model should I place in a FreeCAD document, when it is advisable to split them into separate file?
Should I split every piece into a separate file, and assemble them in a new file? (as basic objects as a simple cube should go into separate file?)

- When I model a relatively complex object through part design, how many object I end up in FreeCAD?
- If I add a secondary object to the same document (a simple bracket or so, which is also created through part design),
is it part of the set of objects in 3D view? So basically I have 40 or so 3D objects in space, from which 38 is hidden? (40 is an arbitrary number, it is how many steps I created the model).

I think this is really the most basic and fundamental question, and I was really too shy to ask it before in public.

Any comments is appreciated.
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quick61
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Re: How many models are in FreeCAD? (very basic question)

Post by quick61 »

arcol wrote:Hi,

I always wondered when I create a model through Part design workbench
(sketch -> pad -> slect a face -> create another sketch -> pocket -> etc, etc), how many models are in FreeCAD?

I mean each step is a new 3D model, and the new step simply hides the previous' step model in 3D view?
No, this is incorrect. When using Part Design in the way you describe, there is only one part. Each step you use to model that part - Pad, Pocket, Revolve, Grove, Transformation... are simply features, (added or subtracted), of that single part.
arcol wrote:If I go to the Edit->duplicate selection, do it create a set of new 3D objects?
Yes.
arcol wrote:Is it advisable to have some independent object in the same freecad document?
You can have as many or as little as you like. It all depends on what your design goal is. If your goal is to design a single part, then there should be only that single part in the document. On the other hand, if your goal is to make a pseudo-assembly of parts, then you would have as many different parts as required to construct that pseudo-assembly.

FreeCAD does not have an official Assembly workbench yet, hence the term "pseudo-assembly".
arcol wrote:I think I miss here the basic concept. I was looking through the freecad document on the wiki, but it did not address this question.

Summary:
- How many independent model should I place in a FreeCAD document, when it is advisable to split them into separate file?
Should I split every piece into a separate file, and assemble them in a new file? (as basic objects as a simple cube should go into separate file?)
Which ever way you want to work. If your using Clones, they must remain in the same document as their parents or you will lose their parametric link. Clones do not link across documents. Other than that, which ever way you are most comfortable working is OK.
arcol wrote:- When I model a relatively complex object through part design, how many object I end up in FreeCAD?
One
arcol wrote:- If I add a secondary object to the same document (a simple bracket or so, which is also created through part design),
is it part of the set of objects in 3D view? So basically I have 40 or so 3D objects in space, from which 38 is hidden? (40 is an arbitrary number, it is how many steps I created the model).
If you make a new independent part within the same document using Part Design, regardless of the amount of features you have used to creat either, you would have 2 parts.
arcol wrote:I think this is really the most basic and fundamental question, and I was really too shy to ask it before in public.

Any comments is appreciated.
The sooner you ask these types of questions, the sooner you will have a more rounded grasp of FreeCAD. I really don't think anyone here would intentionally try to make you feel any less for it. It's only when one fails to make any attempt to understand, or even read the information provided and/or becomes belligerent will you see the claws come out. ;) Asking questions like this... please do not ever feel shy to ask. :)

Mark
Last edited by quick61 on Tue May 19, 2015 4:28 pm, edited 2 times in total.
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r-frank
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Re: How many models are in FreeCAD? (very basic question)

Post by r-frank »

Hello arcol.

The main thing is continuity of information.

Lets look at Solidworks.
In Solidworks you have
> a file containing the parametric info for your solid
> a file containing the editable information about the assembly (which solids? how often ? which position/orientation?)

In FreeCAD you don't have this (at the moment).
ATM I like to model parametric solids in Part/Part Design and the make a "simple copy" and place it an extra file (assembly).
If single part changes, i change the geometry of single part, make simple copy again und use macro to replace/update part in assembly.

This has two advantages:
> it makes the assembly better "readable"
> it uses less PC Power

Because with the strategy we have ATM with Part Design/Part Module, you will reach at some time a moment where it will
become difficult to read and handle the FreeCAD-File.

Maybe this will change with official assembly-workbench ...

Roland
Deutsche FreeCAD Tutorials auf Youtube
My GrabCAD FreeCAD-Projects
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Native german speaker - so apologies for my english, no offense intended :)
arcol
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Re: How many models are in FreeCAD? (very basic question)

Post by arcol »

quick61 wrote: No, this is incorrect. When using Part Design in the way you describe, there is only one part. Each step you use to model that part - Pad, Pocket, Revolve, Grove, Transformation... are simply features, (added or subtracted), of that single part.
Then why it is not reflected in the treeview?
Here is an example:
treeview_how_many_objects.png
treeview_how_many_objects.png (66.3 KiB) Viewed 1426 times
It has three models in it. The big bar, and the two smaller plates.
Why it is not reflected in the treeview? They are at the same level.
So seems like every feature (Pad, Pocket, linear_1046mm, Fillet, Fillet001, Pad001, Pad002) are either an independant object or they are on the same object.
This is where my original confusion comes from.

In reality the three objects are:
Big sheet (purple) in the middle: Pad, Pocket, linear_1046mm, Fillet, Fillet001
brownish rectangular object in front: Pad001 (and Sketch007, which are not dependent on any face)
gray "wing" at the bottom (rectangular object too): Pad002 (and Sketch008, which are also not attached to any face).

And this is the real confusion are:
IF I map the brownish rectangular object's sketch (Sketch007) to the big sheet's front face:
- everything stays in the current position
- the two object becomes a single one
- the purple object (the big sheet) turns also brownish, so the two has the same color
- the treeview does not change

So how do you recognize instantly from the treeview which object are independent,
and which are a simple "feature" dependant to an other object?
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quick61
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Re: How many models are in FreeCAD? (very basic question)

Post by quick61 »

In the example you give in your last post, it does look like you have 3 parts - Fillet001, Pad001 and Pad001. I can not say for sure without seeing the dependency graph. In the example, Fillet001 appears to be made up of the features you mention and that is one part with several features. The other two appear to be separate parts made of of a single feature.

In the screenshot, I have 3 parts. The first has several features like yours and the other two are simple single feature parts.
3Parts.png
3Parts.png (22.81 KiB) Viewed 1409 times
While this might not be the easiest thing to see in the tree view, it is very clear in the dependency graph. Below you can see there are 3 independent parts with varying numbers of features. Std DependencyGraph
3Parts_DepGraph.png
3Parts_DepGraph.png (36.9 KiB) Viewed 1409 times
Does this clear things up a bit? Having the 3 parts in separate documents and then brought together in a new document for the assembly or doing it all within one document is entirely up to you, your preferred workflow and document management.

Mark
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arcol
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Re: How many models are in FreeCAD? (very basic question)

Post by arcol »

quick61 wrote: I can not say for sure without seeing the dependency graph.
Sorry, here is the modell attached.
railing_turnkey.fcstd
(57.28 KiB) Downloaded 22 times
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quick61
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Re: How many models are in FreeCAD? (very basic question)

Post by quick61 »

Yup, you have 3 parts there in a pseudo-assembly. Here is the dependency graph.
3Parts1.png
3Parts1.png (42.95 KiB) Viewed 1390 times
All looks good from here. and to answer your question, "Then why it is not reflected in the treeview?", to me it does seem somewhat clear, and with one quick look at the dependency graph, Tools > Dependency graph... it is very quickly verified. Maybe yes, there could be some sort of automatic separator to make this a bit more clear, but with the availability of the dependency graph, it's not a big priority, if any thing being thought of at all.

If you haven't done so, install graphviz and get accustomed to using the dependency graph tool. It is very useful for a number of things, including this.

Mark
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arcol
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Re: How many models are in FreeCAD? (very basic question)

Post by arcol »

Thank you Quick61.

Why there is a branch in the dependency view?
Eg:
linear_1046mm -> Pocket -> sketch_bottom_hole
linear_1046mm -> sketch_bottom_hole

To me the direct link from linear_1046mm -> sketch_bottom_hole looks bogus.

---

I have an another question. Here is the updated model:
railing_turnkey.fcstd
(90.27 KiB) Downloaded 14 times
The whole project is about to create a railing (around a terrace).

I can not move (either in the Data panel or via Draft workbench -> move tool) the "fillet_top_bar_support" part.
Why is that? It is supposed to be placed on the top of the vertical bar (1250mm in Z direction), rotated 5 degrees (around X axis).

Maybe I should create a dedicated thread to my little pet project?:)
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Re: How many models are in FreeCAD? (very basic question)

Post by DeepSOIC »

arcol wrote:Hi,

I always wondered when I create a model through Part design workbench
(sketch -> pad -> slect a face -> create another sketch -> pocket -> etc, etc), how many models are in FreeCAD?

I mean each step is a new 3D model, and the new step simply hides the previous' step model in 3D view?
I would answer slightly differently than Mark:
Yes, all they are separate models, all the rest is just relationships that defines, how to recalculate the geometry if something is changed.
All the models are stored in the memory, and all are saved into a file (as BRep files). You can verify that by opening a FCStd file with a zip archiver, and then importing .brp files into FreeCAD. It will be completely valid geometry, except that it is dumb (doesn't know, how it was created, and thus not very editable).
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quick61
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Re: How many models are in FreeCAD? (very basic question)

Post by quick61 »

arcol wrote:Thank you Quick61.

Why there is a branch in the dependency view?
Eg:
linear_1046mm -> Pocket -> sketch_bottom_hole
linear_1046mm -> sketch_bottom_hole

To me the direct link from linear_1046mm -> sketch_bottom_hole looks bogus.
linear_1046mm is a linear pattern feature that is derived from Pocket and sketch_bottom_hole so it is linked to both. Changing either sketch_bottom_hole or Pocket will result in an update to linear_1046mm as well. So the model linkage is correct.
I have an another question. Here is the updated model:
[snip]

The whole project is about to create a railing (around a terrace).

I can not move (either in the Data panel or via Draft workbench -> move tool) the "fillet_top_bar_support" part.
Why is that? It is supposed to be placed on the top of the vertical bar (1250mm in Z direction), rotated 5 degrees (around X axis).

Maybe I should create a dedicated thread to my little pet project?:)
You can not move it because in Part Design, every feature is linked to the base (first) sketch in the model. Some day, we will have a body container that all will fit in and be the base of the model and allow it to be moved with more reliability. This is why the most of us create our models in one, or a series of documents and then make simple copies, (part Workbench > Part > Create simple copy and copy those into a new document for assembly/alignment. If your working within the same document, I would use a Draft Clone of that object as it may be beneficial to have the copy parametrically linked, and move the clone while hiding the parent.
railing_turnkey (1).fcstd
(87.69 KiB) Downloaded 9 times
Mark

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