CATIA V5 Creating a Piecemeal Sphere

3D Design Volume Model
1

Hi all

I'm new to CATIA V5, but I'm managing to get by as best I can.

I have to design a storage sphere (with all that it entails: support, taps, etc.). To do this, I need to cut out my sphere as shown in the following diagram : 

I have 2 questions on my mind for the moment: 

  • Do you know a simple way to make this type of cutting? I can create my own pieces of sphere, but I have to enter the values by hand. My pieces are not connected to each other. 
  • During assembly, some parts are identical (as can be seen in the diagram). What would a CAD expert do in this case? He creates all the pieces and then he puts them all together, or does he create one and he does some kind of copy/paste?

Thank you in advance. 

2

Hello

I would tend to create a skeletonized CATPart first with the sphere and these cutouts.

I would design each different part in a CATPart (then I would import with link each cut-out).

As a result, I design in context, so there is no need to position the parts together (fixed).

For identical pieces (the "pattern reuse" command should be useful to you)

This command reuses a pattern (any pattern) that I will create in the skeleton part (rectangular, circular, custom)

 

3

Hello

I don't master all the Catia language, I don't know if I've understood everything well.

I think I did what you said (at least for the first few steps)

  • I created my sphere
  • I cut my sphere with Boolean operations, being careful to take the right dimensions so that "pieces of sphere" don't touch each other
  • I recorded the different catParts. I didn't make all the pieces that are placed at the equator. I was counting on all of them in Assembly Design

You're suggesting that I take all his pieces and reintegrate them into Part Design , right?

For the "pattern reuse" function I didn't know, I'll take a look.

Thank you. 

4

Not to control these parts by a single skeleton CATPart.

The yellow surfaces are the cut-outs, in transparency the repetitions

In blue in parts 01-02-03, the thick surfaces created since the import with link of the cut-outs of the skeleton sphere.

I fixed all the pieces (out of habit) but their position depends only on the skeleton.

 

EDIT: I named the elements and made some modifications in attachment the detail of the graph.


sphere.png
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5

Attached is the definition process

 


sphere.mp4
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6

Here are my 2 Catia docs. 

I have a bit of trouble with the name (product, part, part...), I don't know what it represents concretely. 
The first is the skeleton that I made thanks to your advice. I did it a little differently because I didn't see how to do it any other way. In the end, it seems to work...

For the second one, I don't really know what manipulations I did, but I manage to thicken a part but it's lost in the middle of the tree. My goal is to have all the cuts in pieces so that I can modify some of them, in particular adding feet, stitching etc... But this program is difficult to master.


skeleton.catpart
7

the other file...


squelette_test1_creation_des_pieces.catpart
8

Hello

No PB on your skeleton, that's exactly it

Mine seems simpler because by default our Parts files (CATPart) have a marker on the origin so it saves me from creating the origin point and all the axes (I use those of the marker).

I preferred to use the circular repeat.2 for the top and bottom instances, removing the ones that don't serve rather than symmetries (but that's for the pattern reuse function).

Attached is the video to create the ASS context of the links and the 3 different pieces.

CATProduct file (this is the assembly file, the link pointer to the assembly components, which can be parts or subsets of parts)

CATPart file is the parts file but if you don't associate the parts bodies you can create body assemblies by link or useful constraints for Bi-material parts for example)


import-avec-lien.mp4
9

Thank you, for your explanations, they are very clear. I managed to reconstruct the sphere, I didn't find the symmetry or rotation function (equivalent to reusing a pattern), so I did piece by piece for the polar pieces. Once I have the file with all the parts, can I edit them? I would like to integrate into an equatorial room on two of the supports that will rest on posts. 

In addition, I have problems when displaying the room, they are like spotted. Maybe it's just display artifacts.

Also, when I create a part, for example a sphere, I have a construction line that stays on the object. The problem is that catia considers it as an element in its own right. 

It is in red on the photo: 

10

Hello, indeed the pattern reuse command only works on repeats (custom linear, circular).

The assembly symmetry feature creates a geometrically symmetrical part (i.e. different from the first one).

It's not a display problem, only both modes are visible (surface - solid)

If you hide the skeleton piece and the contents or geometric sets, you will only see the solids, in Catia's default color (grey*). 

Yes, you can modify the parts either from the skeleton (diameter of the sphere, position of the sphere in height // floor, number of repetitions of identical parts, shape of the cuts, etc.)

And add mechanical functions to each unique part (I usually work with the assembly open for skeleton modifications, but since the assembly I open the parts in a new window to add mechanical functions. This is so as not to create links between parts of the assembly).

If I need an external ref I create it in the skeleton and then copy it with link in the room.

I would start by changing the center point of the sphere currently to X0,Y0,Z0 and give it the dimension // on the ground

I will create the reference for positioning and building the columns, as well as the circular repetition of every other piece.

Half shells, you have to deal with it, it's a particularity of CATIA, the same thing is found on cylinders, cones but actually on spheres even if it's a single entity. It behaves to the selection on the geometry as if there were two half-spheres.

11

Thank you for your very relevant answers.

I was able to move forward with the project. I had 2, 3 problems that solved themselves. I created the solid supports directly on the assembly. I couldn't do it on the surface. (I had used volume functions in areal at the beginning and it didn't work well). In the end, I don't know if my assembly is very coherent but it gives pretty much what I want.

On the other hand, I'm stuck again on the stitches. Indeed, when I want to drill part of the sphere at the very top, as there is a circular repeater, the drilling is done on the 3 pieces of the repeater. I understand the problem but, if somehow I manage to remove the link, it will no longer be connected to my skeleton object (I don't know if I'm making myself very clear). 

In addition, I would like to create an excel file that brings together all the values of the sphere AND my parts made on the assembly in order to control the different parameters directly on the excel sheet.

Finally, as it was a bit of a mess, I tried to group my elements into components, it showed me a few error messages about links. I don't know if I did a good job but it seems to work in the end.

12

Hello

For the stitching

Indeed , all instances of a room are identical.

Therefore:

Either you delete the instance that is different, you create a new CATPart from the part (registered as, new name be careful the assembly must not be opened) then you import this new part into the ass and position it in place of the deleted instance. You then have to redefine the link so that the import of the surface points to the right sphere segment //  has its correct blue gear link position. (brown instance or not the right context)

Either there is little difference following the stitching and you consider that it is a re-machining of an instance of the part. Just insert a new (empty) CATPart and then set it to the main body and copy and paste with link the part body of the instance concerned.

Driving from the ass by an Excel table, yes it's possible, but I warn you right away, without a methodology and an explicit naming of CATIA parameters, it can quickly turn into a knot bag.

I advise you first of all to externalize the parameters you want to control in each room and in the skeleton by creating user parameters that control the constraints, dimensions, parameters (to play the modifications.

If everything is robust enough, in a second step since the assembly associate these user parameters with an Excel table.

 

Grouping in components: check if your options (keep the link are still good) and if the constrained option is at tjrs

If not, or in the graph of the ass under Pattern Reuse Assembly Functions, have a yellow triangle symbol. The instances must be deleted and redone.

If you want to control by a table it is important from time to time to save versions of the parts and ASS and play the changes you want.

If you wait until you're done, there's a good risk that it won't work, it's easier to straighten the bar as you go.

 

1 Like
13

If I understand correctly,

  • I'm opening a new Part Design
  • I export the skeleton part as I did last time (publications etc) in this new part
  • I import this new part into the assembly
  • Redefining the link... if I can do it

In the meantime, I managed to do something, but I think it's not right (especially in terms of links).

I copied the piece I was interested in, I pasted it special (break all the links). I managed to make my stitching holes, but I'm afraid that the part is no longer linked to the skeleton. I only hid the linked part, to be able to go back if the manipulation doesn't work.

14

No:

This is a choice to be made, but anyway all imports with a link must be done in the context of assembly.

Either it's a different room with its own plan

Either it is a re-machining

In the first case, we are looking to find the same graph, to be able to modify, to be linked to the correct surface of the skeleton but not to be linked to the original part.

In the second case we want to be linked to the original part and add mechanical functions, (of course a modification of the original instance can lead to a redirection of the references of the changes made after the import with the "update" link).

Case 1 is a new name and new ref in the properties of the file (we then import this part and position it in the desired place in the ass). To redirect the links to the right surface of the skeleton we do a: right click in the graph on the part / component / Define contextual links.

In the window, you select the desired link, the surface of the sphere, then the replaced button and point to the new surface of the skeleton that you have previously published.

 

Case 2 we create an empty part in the ass, we fix it, then we define it on the main body (active Design workshop), we then open the graph of the target instance and we copy its part body then we paste it with link in this new CATPart. The modifications will be made following the linked result, the modifications of the skeleton or the main part will be updated on the linked result.

If you have broken all the links it will not follow the changes of the skeleton.

 

15

Thank you, it seems to work perfectly.

So, can I delete the part I copied, without it affecting, the part I just created? The link is between the latter and the skeleton, isn't it?

16

Yes, if the part you want to delete is a part instance and it's not part of a pattern repeat.

If it is an instance created by a repeat, you must modify under the skeleton repeat (orange dot to delete this instance.

17

I managed to create the different parameters (I haven't tried with excel, but it's already clearer).

I have a problem with the radius of the sphere, when I change it, it can no longer rebuild the sphere, especially at the poles (the lower parts). For the construction I use plans that go through different points (which are already built) but it seems that it can't find them once the geometry changes. I wondered if it was a frequent problem or if I was the :p problem. Anyway, that's a small problem, but I wanted to thank you again for your patience, and for the quality of your explanations.

18

When selecting vertices it is common for Catia to cross along the edge or invert the vertices, we can replace the selection of a vertex by extracting the Extremum (option available under GSD).

I can look tomorrow, put your skeleton file as an attachment.

19

Well, I guess I managed to use the extremum function. I don't know if I used it well but it seems to work pretty well. 

20

There you have it, the masterpiece, in the meantime I have tried other things, including drilling everything (tubing + shell) but without result.

I try to do as you told me. 

What is the advantage of working on the skeleton regarding the stitching?

I create the positions of the stitches on the skeleton, and I make publications that I import into the assembly, right? 

 


assemblage_et_squelette.rar