Test tutorial for Assembly 3 WB

[jpg87]

I think I have got.

Congratulations! The images are of very high quality.
Be careful, however: When the wind blows too hard, the blades move closer to the "flag" position, that is to say that the leading edge (rounded) is facing the wind and the trailing edge (tapered). found towards the rear (therefore towards the mast).

I compared our animations: this comes from my error concerning the inclination of the lights on the toothed wheel of the ogive (which I mentioned on my page http://help-freecad-jpg87.fr/0269_ass_ex_creat_Glob.php "Exchange a component") . This led me to place the weights in the other direction Sorry.

[Kunda1]

I hope you like it, greetings!!!

I don't like it....I love it! Wow!!

[heron]

First of all, I'm glad you liked it, thanks.

I compared our animations: this comes from my error concerning the inclination of the lights on the toothed wheel of the ogive (which I mentioned on my page http://help-freecad-jpg87.fr/0269_ass_ex_creat_Glob.php "Exchange a component") . This led me to place the weights in the other direction Sorry.

I was finishing the assembly when I saw your last videos and I realized this. Nevertheless I decided to continue in this way, because it seemed to me that by turning the weights, the centrifugal force would not push the weights to the right but to the left. I'm not an engineer, just a simple industrial mechanic, but it's the feeling it gives me.
Certainly the blades rotate backwards, that's clear, but it seemed to me that it might also make sense because it would still serve its purpose of slowing down. In the real world, the blades would not rotate that far, the speed would be regulated according to position of the blades (this is my opinion, pure speculation).


I have downloaded the new files from your website. I will take the opportunity to comment some item that may be wrong:

--- The Stator intersects with the BladesSupport and the ExternalBearingRace don't fit with the InternalBearingRace:

error_base_rotor.jpg (38.81 KiB) Viewed 2950 times

It needs 0,9 mm offset. I think you chose a wrong Element ExternalBearingRace:

base_rotor_offset09.jpg (32.01 KiB) Viewed 2950 times

--- The Warhead intersects with the BladesSupport:

crash_warhead_rotor.jpg (31.2 KiB) Viewed 2950 times

--- The Warhead intersects with the OjiveGearWheel:

crash_warhead_gear.jpg (21.48 KiB) Viewed 2950 times

There are several possible solutions, I leave it in your hands.

Regards.

[jpg87]

I will take the opportunity to comment some item that may be wrong:

Horror! All your remarks are perfectly justified. I was so focused on the assembly that I forgot the most basic of the controls. Hope to have time at the end of the day to download the corrected files.
My humble apologies.

[jpg87]

I hope I haven't forgotten anything.
Sorry again for those who used my wrong files!

vue_corr.png (58.84 KiB) Viewed 2812 times

[bozzo]

@jpg87 Thanks for the tutorial website, It's exactly what I was looking for!

Some questions on the workflow. In the tutorial on linked geometries where you create the well, you copy the master sketches to individual bodies. If I understand correctly this approach works because the copied sketch links all constraints via formulas to the original sketch.

I noticed that if the sketch was not fully constrained when the copy of the sketch in the body is made the copy is not really linked to the master sketch. This is easy to fix, always fully constrain the master sketches (maybe worth mentioning in the tutorial)

What would be a good iterative workflow when you don't know all the elements of the design up-front? Always create new master sketches, never modify existing ones? Any better approach?

for example, I discovered the floowing is not a good approach: If the original geometry is modified by adding more elements these do not propagate automatically to the copies. making the copy again inside the existing sketch, I get a fresh copy of everything from the master sketch, so most of geometry is duplicated.

Also, if I do need to modify an existing master sketch, how do I safely propagate the change through the copies?

Again, thanks for the tutorials!

[jpg87]

Hello,
Thanks for trying my tutorials and providing insightful comments.

If I understand correctly this approach works because the copied sketch links all constraints via formulas to the original sketch.

This is the goal, to link basic geometries so as not to have to reconstruct too many things, as well as dimensions whose modifications will be reflected automatically. It is obviously possible to supplement with parameters in spreadsheets or DynamicData.

I noticed that if the sketch was not fully constrained when the copy of the sketch in the body is made the copy is not really linked to the master sketch. This is easy to fix, always fully constrain the master sketches (maybe worth mentioning in the tutorial)

I just gave a test run with the latest version of FC (https://github.com/FreeCAD/FreeCAD/rele ... -x86_64.7z), it seems that this problem no longer occurs. But your proposition is perfectly correct.

What would be a good iterative workflow when you don't know all the elements of the design up-front? Always create new master sketches, never modify existing ones? Any better approach?
for example, I discovered the floowing is not a good approach: If the original geometry is modified by adding more elements these do not propagate automatically to the copies. making the copy again inside the existing sketch, I get a fresh copy of everything from the master sketch, so most of geometry is duplicated.

My experience does not allow me to decide, especially since we all have a more or less personal approach (I am only experimenting and sharing what I think is interesting in what I understood).
However I would avoid modifying the geometry of my master sketches at the start of the project so as not to take the risk of weakening the model.

Also, if I do need to modify an existing master sketch, how do I safely propagate the change through the copies?

If I don't have a clear enough idea of ​​my project at the start of my design, which is most often the case, I would tend not to put too much geometry in the first master sketches and then add new ones. master sketches as the project needs. These new sketches may contain copies of the first ones and supplement them.

These answers of course only reflect a personal point of view.
Anyway, thank you for your very interesting questions.

[bambuko]

I am following examples on your webpage (thank you very much for creating it!),
trying to familiarise myself with Assembly 3, and...
the first question (clarification, please) I have is with terminology.
Here:
http://help-freecad-jpg87.fr/0251_ass_e ... ssieux.php
you are talking about "reference" and "complementary" components.

This terms may have been defined somewhere on your webpage (if so I do apologise for missing it), but just to be absolutely clear:
"reference" - are fixed?
"complementary" - have relationshio with reference components?

The second question I have is this:
Your examples all have components in separate files, I presume I can also have them in the same file?

[jpg87]

Hello and thank you for your interest in my website.

This terms may have been defined somewhere on your webpage (if so I do apologise for missing it), but just to be absolutely clear:
"reference" - are fixed?
"complementary" - have relationshio with reference components?

The "reference" is as you understood it the immobilized part in the kinematic equivalence class concerned (sub-assembly).
In a global assembly, it is the kinematic equivalence class which plays the role of support, if not the one to which the greatest number of the others refer.
If you haven't already done so, you can visit the pages
http://help-freecad-jpg87.fr/020_ass_outils_contr.php
http://help-freecad-jpg87.fr/021a_ass_principe.php#

The "complementary parts" are the other components of the same kinematic equivalence class, or the other kinematic equivalence classes of a global assembly.

Note: the examples I have chosen on this website all relate to "mechanisms", that is, systems in which some components remain mobile in relation to others. There is therefore in general (simple cases) an entry movement and an exit movement.
BUT nothing prevents using an assembly workbench to position a set of components that do not include any functional mobility, for example furniture in a home (this is also the case by definition for components of the same kinematic equivalence class in a mechanism).

Your examples all have components in separate files, I presume I can also have them in the same file?

Of course ! see the "hypnotic" example on this page
http://help-freecad-jpg87.fr/025b_ass_ex_creat.php

[bambuko]

Thank you again jpg87

I am only interested in kinematic assemblies (the rest I can easily handle without assembly workbench).
I have so far done it using sketches and spreadsheet, but it has limitations... so I look forward to trying Assembly 3.
My plan is to take one of my existing models (steam locomotive) and make kinematic assembly of the motion (connecting rod, coupling rods, valve gear etc).

So your examples are very pertinent to what I am trying to do!

I presume (will try it soon) that I can "immobilise" a part that has a variable dimension driven from the spreadsheet - so that it is immobilised but can be "driven" by this variable dimension.

I will look at hypnotic now