the other file...
squelette_test1_creation_des_pieces.catpart
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
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:
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.
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.
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.
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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.
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.
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?
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.
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.
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.
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.
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
Hello
The advantage of creating the implantation of the stitches in the skeleton is to direct the links only from the parts to the skeleton, not to have links between parts.
I looked for the stitching, there are two different pieces in the same place (it must not be normal)
For the cutting of the stitches there is a simpler integrated into the skeleton.
To make your tubes, look when you make an extrusion of a sketch, try the option (Thicken).
I attached the images as well
piquages.7z
I made my bearings on the skeleton. I created publications that I copied with links in the different parts on the assembly (shells + tubing).
I use these markers to make my holes in the shells, it works perfectly.
I make a circle for my tubing, placing it with these markings, and doing the extrusion to the next one, it gives me an error message "you cannot specify a limit of the type "until the next" for the first component of the current part body"
I have the impression that I want to make my parts separate but still connected to each other.
Hello, it's normal, the extrusion you want to do is the first volume operation in your file, so there is no "next" (meaning to go to the next geometry (solid) in one direction).
In your case you have to take up to the surface and select the surface of the imported sphere with link in the geometric set above.
EDIT:
Your skeleton is not in the right place, it should be at the top of what it is piloting, it is stored in the sphere component, it would be okay if links didn't come out of the sphere component to drive other parts.
I advise you to be rigorous, you have to rename the elements with an implicit name (in some time it will be difficult to remember that Symmetry .3 is the spherical surface of the " Central Lower Pole").
Be careful, there are several inactivated formulas, if it is not voluntary (controlled) they must be destroyed.
There are also 6 default parameter tables?
Many imports with links are found out of context of creating their links.
Many formulas refer to the same parameter , in these cases there is the " Equivalence " function which is very handy.
http://www.lynkoa.com/tutos/3d/catia-v5-fonction-equivalences
Thank you for all these tips.
In the meantime I had managed to solve the problem. I actually redid almost all the assembly because by editing the formulas (I think) I broke the links with the skeleton. It seems that the problem has been solved. All I need to do is make the bracing between each post and if I have the courage, the access staircase (it may be a different story).
I could not be more aware of the approximate rigor of my Catia blend. By dint of experimenting I start to understand the links between the pieces and it starts to work the way I want it to. The problem is that I started the play without really knowing what I was doing... So, it's not very rigorous.
I'm going to refrain from moving my sphere component in the folders, I'm afraid that the assembly won't recognize it anymore and that I'll have to start all over again.
I also deleted the parameter tables, I saw in the meantime how to do it. At the end, I'll create all my parameters in the skeleton file and they'll drive both the dimensions of the skeleton and the assembly. I think the method is a bit boring and not approved, with a list of parameters as long as my arm, but I tested 2, 3 times, it seems to work. I think I noticed the relationships not to be touched on the assembly, those that concern the dimensions of the skeleton. I will be careful not to touch it.
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Indeed if you moved the skeleton part under the head assembly you would have to redefine all the Contextual links