Assembly design Catia V5 Circular repetition of a sub-assembly around a rotation axis

Out of category
1

Hello friends: 

I try to repeat a sub-assembly (please consult the attached figure) around a motor axis, in order to fix my sub-assembly 3 more times

in its place (green connection _ see photo) 

I tried a first time with the compass while selecting the subassembly, but the rotation was wrong, it was done from the base of the subassembly and not from the axis of rotation (see red comment on the photo). I find this normal because I couldn't select the axis around which the subset is supposed to rotate. 

Can you please tell me how I can properly run the desired subassembly? 

Thank you very much for your assistance,

Sincerely,

Manel

 


catia.jpg
2

Hello

If the shape doesn't allow you to detect an axis, nothing prevents you from creating it (a straight line does the trick very well).

Another practical solution if you have a circular repeater in your green room is the re-use of a pattern control.

3

Hello;  

Thank you for your answer.

I tried the first solution but it didn't work, most likely because I didn't understand how to select both the axis of rotation and the subset to want to rotate. 

The green piece is fixed. I must not duplicate it, nor run it.

At the beginning I created an axis on the motion transmission shaft or motor shaft (see image) 

I selected the axis created with the subset and rotated using the compass.

I found that it is the engine with the sub-assembly that ran (both of them), which is not the goal.

Then I created a rotation axis in the green room. I repeated the same thing, this time it was the green part and the subset that rotated, which is also not the goal.

Can you please tell me how I should use the rotation axis, with the subset and the compass to just rotate the subset around the axis? 

Thank you again for your time and help.

Sincerely,

Manel


a3.jpg
4

If you want to rotate around an axis, the compass must be on this axis in both your copies, this is not the case.

but maybe I don't understand what you're trying to do, it's probably clear to you but if you hid everything that isn't useful and you showed how your assembly constraints are it might be + for me

 

Edit : in my example the Part1 is fixed, the Part2 constrained, the Part3 (copy/paste the Part1 in position).

I am careful that nothing is selected, I take the compass by its red square, I approach the axis when it aligns with it I let it go.

I then select the Part2 and then right-click on the compass Edit after following the axis of the compass coincide with the axis drawn, I enter the value and rotate.

5

Thank you! I managed to run my subset correctly. I put the compass on the axis this time and followed the rest of the procedure as you told me.

In the diagram attached the constraints of the subset to be rotated . I'm going to attach the constraints of the green piece.

Have a nice day 

Yours sincerely,

Manel


a7.jpg
6

Attached are the constraints of the green and yellow part, these two are supposed to be fixed.


a8.jpg
7

Note: Before rotating the subset (copied from the original),  you just have to remove the constraints of the latter before rotating; if not, it will follow the meaning of its (father or original subset).

8

When I look at your screenshots, not everything is constrained, (16 constraints for at least 15 components, ideally there should be 45, or even one less per piece of revolution like the screws if the orientation of the head doesn't matter). You haven't mastered the position of your assembly in space.

If you design in position, it doesn't matter, but if you design parts that will eventually have to be implemented in other assemblies in different positions, it's more efficient to master this position in space from the design of the part or sub-assembly.

For example, for a screw, it is customary to have designed the supports under the head to coincide with the plane XY and the axis of rotation of the screw to coincide with the Z axis of the part (the head in + Z, the body filtered in -Z)

And all our screws are like this, which allows us in an assembly not to select the geometry of the screw (it can change over time if specific screw) but to select the Z axis and the XY plane, they will never be modified or deleted so the assembly constraints will be stable over time, if we rely on the geometry there is a high risk loss of reference following a modification (e.g. a screw hole on which we have centered and which turns into an oblong hole to facilitate assembly, the concentricity will not like.

 

To control the position in space, the first constraint must be a fixity (by habit I fix the part that serves as a support, then successively the following ones in the order of assembly) always of the part to be positioned on the part that positions.

 

CATIA does not display the origin of the assembly as you can have in a CATPart (three planes or the absolute coordinate system).

When you import the first part, depending on whether it was designed in space or stored on its origin, you don't really know where the origin of the assembly is.

A trick is to first import an empty CATPart that you fix, then the support part that you will constrain as needed on the empty part.

Once done, the empty part and all the constraints are removed and then the part (support) is fixed.

Then we constrain the following ones in the order of assembly (BestPractice tjrs of the part to be positioned on the one that positions).

The readability of the constraints in CATIA by default is not the most meaningful and can quickly become cluttered.

Don't hesitate to change the order or group the constraints

9

On your copy a8.jpg

The pipe and fitting parts are effectively fixed inside the sub-assembly (Product1).

But if your sub-assembly (Product1) is not itself fixed or constrained at the head assembly (Pump assembly), there is no guarantee that the assembly (parts + hose) will remain in place if you use the geometry of one of these two parts to position others. 

10

Thank you very much for this explanation and the time you have taken to get my attention

on the control of constraints in space.

I have already fixed all my sub-assemblies, as you told me.

I suffered a lot from the problem: after having done the assembly of a sub-assembly X, the slightest intervention on a sub-assembly Y linked to X, destroys the assembly of X and I redo the work etc....

Now I understand why.

I'm going to review the other constraints, see what's missing.

A question please: Can I fix a part that is supposed to rotate? 

LIKE the axis of the motor for example.

Thanks in advance


a10.jpg
11

I would say yes if, in its assembly no need to rotate it .

In order to be able to use the axis and assign an angular stress to it if necessary in a head assembly, it will be sufficient to soften the sub-assembly. (the typical example and the rod of a cylinder by default there is little chance that the rod stroke will correspond to the need when the cylinder has been imported , it is sufficient to soften the cylinder sub-assembly to be able to stress the rod and its clevis at the head assembly independently of the original constraints of the sub-assembly). 

Edit: 

12

Okay, thank you very much!