If you want to constrain the reference parts contained in the "Component" you have to soften the component, then you can select the elements to constrain.
See attached video
assouplir.mp4
assouplir.mp4
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Hello
It may be necessary, in fact, to constrain the reference parts contained in the "Component". But, I'm not sure yet.
In fact, I thought that using instantiation with the optimized point-2 directions copies on the coordinate systems (axis system) of the parts of my mechanism. The 3D markings (added in the "component") would follow the movement of the parts of my mechanism.
Questions:
1) Isn't it possible to use optimized copies? Why didn't you use them?
2) I'm not sure I understood the interest of the relaxation function. What I understand is that this allows you to put different and independent constraints for each of the parts contained in the "component" Benchmark. Is that the case?
Obviously, separating 3D landmarks doesn't seem that simple...
Thank you in advance for your help.
The best practice would be in assembly, to have a part. Catpart (skeleton).
This part schematizes the mechanism in dimensions, positioning, settings.
On schematic elements (plane, line, etc., coordinate system) we instantiate the 3D coordinate systems (optimized copy).
Then the parts of the mechanism are created in the assembly (which are built on the basis of the published elements of the skeleton).
That's the skeleton method.
like this in the assembly the parts are dissociated from the marks (we simply hide the skeleton part.
You write:
In fact, I thought that using instantiation with the optimized point-2 directions copies on the coordinate systems (axis system) of the parts of my mechanism. The 3D markings (added in the "component") would follow the movement of the parts of my mechanism
If you have these axis systems, the simple + is to constrain the parts marker 3D.Catpart (assembly constraint Catia marker on marker) and it's done. (if these 3D coordinate parts are grouped together in a catproduct or component, it must be relaxed, this is the simplest + way to constrain the coordinate parts on external elements. (the axis systems of the parts of your assembly).
In short
- If it's a kinematic diagram that you don't have the geometry of the parts. I will create a skeleton part where I instantiate the 3D landmarks. (advantage we develop the kinematics and then we will build the parts of the mechanism in the context of assembly based on the skeleton)
- If the parts exist and can be constrained together in a Catproduct , I will create a component in this catproduct in which I insert the 3D reference parts that I position in relation to the axis system of the parts of the mechanism. (kinematics is provided by the geometry of the parts of the mechanism, so we can easily use standard components or components belonging to another assembly)
In both cases, the 3D coordinate systems are separated from the mechanism.
Case 1 in the skeleton room
Case 2 in the Catproduct or Landmarks component.
Thank you Franck for this detailed and very interesting answer! It's worth +10 to me!
Yes, I'm reformulating, you mention 2 methods:
Method 1: A global skeleton
In this method, the mechanism is built from a single skeleton that is contained within a part. Then, the parts of the mechanism are built from the skeleton. Here, I am missing a little bit of elements to fully understand this method. Hence my question at the end of this post.
Method 2: Basic method without skeleton
In this method, the mechanism is built by an assembly of parts and the parts are constrained together from elements that belong to the volume.
For information, however, it seems to me that there is a third method which is a kind of mix between the two methods, namely:
Method 3: One skeleton per room
In this method, the mechanism is built from parts that each contain a skeleton (which is materialized by a geometric set that contains the wireframes). The parts of the assembly are constrained at the level of the different skeletons. We then obtain that a wired and constrained assembly. The last step is then to add volumes.
Conclusions/questions
For the moment, compared to what I have already done (using method 3), I will go for solution 2 that you told me, namely;
1) Create a "component"
2) Darken the "component"
3) Add the 3D landmarks by instantiating optimized copies based on the skeletons of my different parts.
If you have these axis systems, the simple + is to constrain the 3D marker parts. Quote Franck
--> here, I don't understand why we don't use the optimized copies that we took a long time to define properly.
For method 1, for my information, how are the constraints between the wireframe elements (plane, line, ...) constructed?
Thank you for your ideas and sharing on this discussion, which was very constructive for me.
Good evening
1 ) because it avoids increasing the number of publications (the more there are, the less it is readable by another user) moreover Catia has the assembly constraint Benchmark on marker it's very practical a single constraint and the part no longer has a degree of freedom.
2 ) these are the construction constraints (e.g. a straight angle // has a curve) it implicitly has a coincidence (// at its starting point), a coincidence (// at its support plane) an angular stress (// at the ref curve) and so on.
In the video the connecting rod length (sketch) is constrained coincident one point on the vilo, one point on the cylinder axis, one side for the length.
3rd Method:
Less practical because you have to look for the publications inside each piece unlike method 1 where it is the skeleton part that centralizes them.
In fact I use a 4th method (because in our projects we have a lot of standard components whose geometry is already defined and not modifiable "standard".
I create a skeleton part that schematizes the mechanism but only serves to position the parts in the assembly
Inside the parts to be designed, I create the construction skeletons.
I re-publish the useful elements of these skeletons at the higher level (the CATProduct), so we don't look for them they are directly usable in the CATProduct publication container.
If an element is common to 2+ parts, I build it in the positioning skeleton instead of the parts and re_publie it in the catproduct.
I'm trying to set up the "Component + Easing" method.
I think I'm starting to understand why you didn't use optimized copies much in this case. In fact, the reason is that, when you do this method, you have to create as many parts in the component as there are 3D guides you want to add. However, these 3D coordinate systems are centered on the parts that are added and there is no need to position the 3D reference body at a particular position on the part.
Questions:
1) In the "soften" video, why did you attach the first 3D marker you added?
2) In this method ("Component + Flexibility"), the point that bothers me is the fact that we are forced to add constraints to position the 3D coordinate systems but which do not correspond to the functional constraints of my mechanism (i.e. related to kinematic links).
So, I think I'll try the following method instead:
- adding a 3D cue in each part of my mechanism using an optimized copy
- separate the added body by putting it in an ordered geometric set so as not to mix the functional bodies of my mechanism and those related to the dressing. This also has an advantage, which is that in mecha a coordinate system is associated with a solid (therefore with a share in CATIA).
On the other hand, with this way of doing things, I will still have a problem. When 2 instances of the same object are present in a mechanism (for example a parallel robot that has several times an identical arm), if we add 3D cues on one of the arms of the mechanism, all the other arms will also have a 3D cue. However, often it is interesting to add 3D guides only on one arm to see the marks that have been used for the parameterization but not on all the arms so as not to overload the figure.
What do you think of this way of doing things and the blocking point mentioned (inevitable copying of all the 3D markers on all the instanced parts)?
Thank you in advance for your help.
1 ) I fixed the "component" (not the first reference part) I don't leave any unconstrained elements in an ASS.
2 ) We can always group the constraints related to the coordinate system in a group.
I noticed that on your files I can't coincident the coordinate system on another coordinate system? may be related to the fact that I work in Normal mode (the hybrid mode is locked ADMIN) so I can't test. so if it doesn't work 3 constraints to position each marker, it's not practical!
3 ) You write:
What do you think of this way of doing things and the blocking point mentioned (inevitable copying of all the 3D markers on all the instanced parts)?
It is inevitable that the instance of a piece is the piece, so everything that is visible is visible in all instances.
You can still go through a variant (the simplest in your case copy / paste with link of the geometry of the part in a new part) and instantiate the marker in this part.
If an exact nomenclature is needed, the part must be superimposed (hidden) on the variant and excluded from the nomenclature.
Super. Thank you for your latest information.
1) Info:
For the moment, I believe, even if it's not ideal, that I'm going to create my 3D landmarks in the parts associated with my mechanical parts by optimized copies and I'll make a version of my "mechanism" product with landmarks and one without 3D markers.
I find, in fact, that redoing constraints for each of the "3D Landmarks" parts is a bit long.
2) Question:
I'm in the process of setting up my benchmarks. On the other hand, I just realized that I didn't manage the settings well so that I could adjust its dimensions. Indeed, if I double the length of my axes, the volume of my axes no longer follows and my coordinate system is no longer orthogonal.
2.1) Can you remind me how you managed the setting of the marker?
It seems to me that you used:
- the length of the axes;
- a ration for arrows.
On the other hand, the videos don't show how you defined them. Can you add a short video on this point?
2.2) Then there is the step of setting the setting when instantiating an optimized copy. Can you tell me how to define the consideration of parameters when defining an optimized copy?
By the way, my feeling about taking parameters into account during the optimized copy seems to me a bit "gimmicky" and much less important than the definition of the reference elements involved in the positioning of a body. But, my eyes are still perhaps too naïve on this subject....
Good evening the best put the file I will tell you what is wrong
Already in your screenshot you don't embed the relationships in the optimized copy which means that once instantiated it can't be modified and follow since the relationship (ratio is not embedded).
I'll make a video tomorrow for the "publication" of the parameters in an optimized copy.
While remaining at level 1 of optimized copies, it is very useful imagine that the copy is made to instantiate the housing of a shaft (drilling, shoulder, circlips, input chamfer, etc.) the user can change these values before the copy is rebuilt.
At level 2 we will make sure that the copy finds this information directly in the tree.
The level 2 copy adapts to its environment.
Great Franck! Thank you very much for your help and information.
By the way, the selection of points comes the arrows on the numeric keypad is great.
Otherwise, I tried to roll out your tutorial.
I'm missing two stages at the end.
1) "Sketch.1 we have to redirect the formula to the embedded equivalence" Now, can you add some info to me because for the moment, I haven't understood yet.
2) Can you show me where you set the ratio for arrows?
Thank you in advance for your help
2) I didn't change anything, it's you who defines it in the diamis of the sphere by a formula that relies on the parameter of "equivalence.1" in your file and then in the arrow sketch by the external ref on "projection of the silouhette line of the sphere and ratio by formula on the parameter of "equivalence.1".
1 ) One of the disadvantages in Hybrid mode is that you can't reorder as you want (it's made for). equivalence.1 cannot be reordered in the geometric set, I had to recreate an equivalence.2 by being active on the geometric set so the formulas must be redirected to the equivalence parameter.2
Then move to the geometric set to be embedded in the copy.
Edit: Redirect, we select the equivalence parameter in the text of the formula.1 ('Relations\Equivalence.1\Value') and then we point in the graph to the equivalence parameter.2
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Sorry Franck to ask you again for these same steps but it's been 3 times that I've reread your word document and the following two remarks:
1 ) One of the disadvantages in Hybrid mode is that you can't reorder as you want (it's made for). equivalence.1 can't be reordered in the geometric set, I had to recreate an equivalence.2 by being active on the geometric set so the formulas have to be redirected to the equivalence parameter.2
2) I didn't change anything, it's you who defines it in the diamis of the sphere by a formula that relies on the parameter of "equivalence.1" in your file and then in the arrow sketch by the external ref on "projection of the silouhette line of the sphere and ratio by formula on the parameter of "equivalence.1".
AND I still don't understand the remark:
and I still don't understand the remark "Sketch.1 you have to redirect the formula to the embedded equivalence. Then move the formula under the container of the geometric set"
Even if I already have an Equivalence.1 in the relationship tab on my part 3D coordinate system, do I need to create a new equivalence in the geometric set of my 3D coordinate body body?
It would be great if you could give me a new detail of this step (via a short video and by momentarily going back to hybrid mode) and I apologize if I'm a bit heavy at the time.
Thank you in advance for your help.
Hello
I can't put myself in hybrid mode, it's locked by CATIA ADMIN, it's too complicated to transform a hybrid design into normal, and for the type of parts we develop, it's too restrictive, we decided to forbid the use of hybrid mode to CATIA users and so to be like the others, I don't have an administrator account.
No, it's not essential to move the equivalence and formulas unless you want to be able to modify your 3D respers after their instantiation in another CATPart, if you instantiate them in the same CATPart, no PB
Redirect the formula (redo it if you prefer) currently your formula is "value of the parameter of the equivalence1 / 10."
It has to be "value of the parameter of the equivalence2/10."
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Super! Thank you very much for your help. I think I have finally understood the last remarks. It was a question of putting the equivalence in the ordered set of the main body so that the equivalence would be preserved by copying the body.
I have finished my bearings. I have copied them here.
In fact, I have created 2 following guides that one wants to use the method:
1) Method 1: add a "3D cue" body in each part of my mechanism using an optimized copy
--> In this case, the share contains the optimized copies that can be used.
2) Method 2: adding a 3D coordinate system to a component that is relaxed in order to be able to put independent constraints on each of the parts of the component.
--> In this case, there is no need for optimized copies since we copy the part directly.
Questions:
1) Can you check me on the two reference parts?
2) When we do method 2, in fact, we can still separate the constraints well. So, I go back to my previous preconception and I find this method not bad. By the way, how do you constrain the landmarks: 2 coincidences on two axes are enough, aren't they?
Thank you in advance for your help and see you soon.
rep.zip
Good evening:
1 ) I'm looking at tomorrow
2) yes two axes is enough but in normal design it is enough to constrain one coordinate system on another (a single constraint is enough) it doesn't work in hybrid? (you have to select the marks in the tree not on the geometry)
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Hello:
I looked at the files:
On the optimized copy "3D Coordinate System-2 directions". the origin is 10 mm in (Z)? (maybe that's what you want).
On the "Repere3DS2_Seul.CATPart" file
I will publish the axis system of the 3D coordinate system to facilitate the implementation of constraints if of course the coincidence of reference / reference system works in hybrid.