Catia V5 Drafting Mode
Catia V5 Drafting Mode
(OP)
Hello Catia users
My name is John. I work in an Aerospace facility. This company recently purchased Catia V5 revision 18 or 19 I don’t recall off hand. For my questions this change in revision levels should have no effect. I have been using 3-d modeling since 1998 (college) and 2000 (industry). In industry my predominant use was in UG and Solid works. I like all other users in different software packages look for similar features to accomplish engineering tasks and projects.
After completing a product assembly, can I complete the following? (Switch to drafting workbench)
1. Create view 1 with all components shown.
2. Create view 2 with components hidden, not shown, inactive or whatever terms may be used in Catia.
Modify the assembly (product) remove components, modify geometry etc… Rebuild product and drawing to reflect changes.
3. Can I maintain view 1 rebuilt reflecting these changes?
4. Can I maintain view 2 rebuilt reflecting these changes?
An example would be if I had a top die assembly and a bottom die assembly.
View 1 = top and bottom dies shown.
View 2 = top die assy. components shown only.
View 3 = bottom die assy. components shown only.
5. In the drafting workbench under each view can I view the entire tree of components used to create each view? Select, show hide etc….
After modifying the product I should be able to maintain the links for all 3 views and have them update accordingly. Right now I create view 1. Hide components for view 2 (in product mode) and then on my drawing view 1 now falls apart showing of course view two. My solution is it isolates views after creating them but this really sucks. Please help.
Thank you
John
My name is John. I work in an Aerospace facility. This company recently purchased Catia V5 revision 18 or 19 I don’t recall off hand. For my questions this change in revision levels should have no effect. I have been using 3-d modeling since 1998 (college) and 2000 (industry). In industry my predominant use was in UG and Solid works. I like all other users in different software packages look for similar features to accomplish engineering tasks and projects.
After completing a product assembly, can I complete the following? (Switch to drafting workbench)
1. Create view 1 with all components shown.
2. Create view 2 with components hidden, not shown, inactive or whatever terms may be used in Catia.
Modify the assembly (product) remove components, modify geometry etc… Rebuild product and drawing to reflect changes.
3. Can I maintain view 1 rebuilt reflecting these changes?
4. Can I maintain view 2 rebuilt reflecting these changes?
An example would be if I had a top die assembly and a bottom die assembly.
View 1 = top and bottom dies shown.
View 2 = top die assy. components shown only.
View 3 = bottom die assy. components shown only.
5. In the drafting workbench under each view can I view the entire tree of components used to create each view? Select, show hide etc….
After modifying the product I should be able to maintain the links for all 3 views and have them update accordingly. Right now I create view 1. Hide components for view 2 (in product mode) and then on my drawing view 1 now falls apart showing of course view two. My solution is it isolates views after creating them but this really sucks. Please help.
Thank you
John





RE: Catia V5 Drafting Mode
Hope that helps.
CATIA V5 R20
PC-DMIS 2011 MR1
RE: Catia V5 Drafting Mode
Your company made a big investment in CATIA. Hopefully they also purchased some training inorder to maximize their investment. If not, your company is wasting alot of time and money! In class, you will learn how to do all the steps above. (just let the instructor know this ahead of time)
The company that sold CATIA should be able to come to your office and show you and your design team how to accomplish the steps you have listed. It would be much better to have someone show you the process in person and answer any other questions. This would be more efficient then relying on forums such as this one.
Jack
RE: Catia V5 Drafting Mode
Thanks for the advice. We had five of us in a short training class. By Friday afternoon the other four were literally sleeping. I was the only employee that was awake. Since they all feel the Product Mode is a waste of time they caught up on needed rest. They build each component of an assembly in one part file (multiple bodies in one part file) using translate, rotate etc... Any change to a part creates big issues and all of the drawings are falling apart. Future employees will have no idea how dies were cut since rebuilding a drawing shows a completely different drawing of the current showing components. My questions are to educate myself since I enjoy learning and doing things correctly. In the future if I’m required to clean up the mess that is being made I want to have a plan of action. Otherwise it’s good practice and education for my future career path. I would not set up a cad system for a 50 million dollar corporation based on tips and tricks from a website. The people on this site in many instances have clever insights and methods for solving problems. Again thanks for the advice.
Thank you Dasalo for the help you provided in your post. Scenes were used many years ago in other packages. So this helped put me on the right track.
John
RE: Catia V5 Drafting Mode
Thanks for the reply, and I'm glad to hear you and your co-workers did get some training. I suggest you get in touch with your instructor and ask him/her for their suggestions to your drawing questions.
Scenes are definitely one method to show different components of an assembly. But, Overload Properties is another method that might be better in your situation to show/hide various components in different drawing views. For your co-workers that insist on making assemblies with Bodies in a Part, Modify Links can be used instead of Overload Properties.
RE: Catia V5 Drafting Mode
Thanks for the help.
For your co-workers that insist on making assemblies with Bodies in a Part, Modify Links can be used instead of Overload Properties.
I tried this Part Modify Link in the drafting mode but it is grayed out. Maybe I don't have the rights to acomplish this ?
John
RE: Catia V5 Drafting Mode
Start with a normal drawing containing several views of a 3DCATPart. The top section of Modify Links will show you all the Bodies that are "pointed" (currently used to define the view). You can select one or more Bodies and Remove them if there are Bodies you don't want to see in that view.
Adding more Bodies isn't that easy:
1. right-click on the view and select Modify Links
2. change window to the parent 3D CATPart
3. select the Bodies to be added to the view
4. return to the drawing window, and note the lower section (3D elements to add)
5. click the ADD ALL button to move them to the Pointed Element section
6. click OK
7. Update the view to see all the pointed elements in that view
Use Apply Links To to copy definition to other views
RE: Catia V5 Drafting Mode
RE: Catia V5 Drafting Mode
RE: Catia V5 Drafting Mode
I will add my notes on this as well.
In regard to scenes: I have used these and would just mention that when I added a new detail I WAS able to include it in an existing scene (it was mentioned that a new scene would need to be created). Edit the scene you need the new item in and unhide it from the tree. At least I've gotten that to work in our version, 5.20.
When we create views, we use the method mentioned by Albigger - selecting the individual parts from the tree. It's pretty simple to modify the links of those views and add/remove parts as needed later.
Brad
RE: Catia V5 Drafting Mode
I have been all over the internet and ask various catia "experts" about adding a new componet to a scene that was added to the model. In your previous post you mentioned that all you had to do was unhide the part from the tree. When I am in the enhanced scene workbench I dont see the new componet in the tree as it appears in the assembly workbench. Is there anyway that you can elaborate on this? If it is possible to add new parts to an existing scene, it would save me and my office so much time and effort.
Thanks,
Travis
RE: Catia V5 Drafting Mode
After looking into this, I've discovered that when I was creating the enhanced scenes I was using the 'Partial' option under the Overload Mode (this was the default) - even though I use everything in the assembly, it's just the option I chose when I created the scene. When adding a new item it does appear in the tree and in the scene. However, if I create a scene and choose the 'Full' option for Overload Mode any new items do not appear in the tree - as you have seen. I don't know of a way to switch from Full to Partial once the scene has been created, or how to get the new item to show up so I'm not sure what help this will be for any existing scenes - just that for future reference the Partial option could be selected to avoid this issue.
Brad
RE: Catia V5 Drafting Mode
CATIA V5 R20
PC-DMIS 2011 MR1
RE: Catia V5 Drafting Mode
A description of the two from the above link:
Overload Mode Partial: The scene will only overload attributes for a few products and modifications to the main assembly of those attributes not overloaded in the scene will impact the scene. Overload Mode Partial favors performance as long as you don't overload too many attributes.
Overload Mode Full: All attributes supported for overloading of each element of the assembly (under the products selected at scene creation) will be overloaded by the scene. Products overloaded by the scene will henceforth not be impacted by modifications to the main assembly regarding attributes supported for overloading. Overload Mode Full favors Enhanced Scene independence from the Assembly.
Something I'll look into further when I have more time.
Brad
RE: Catia V5 Drafting Mode
RE: Catia V5 Drafting Mode
Weavedreamers idea for converting them could work. Is it possible to change the link of a drawing view from one scene to another without recreating all the dimensions and notes and all the fun drafting stuff required on a drawing?
-Travis
RE: Catia V5 Drafting Mode
RE: Catia V5 Drafting Mode
I thought the same thing so I made new scenes and with the same name (copied & pasted)and my drawing dropped all the links and forced me to recreate my 9 page drawing.
-Travis
RE: Catia V5 Drafting Mode
Another way to hide and/or modify part properties in drafting without affecting its links is to right click on the display view frame and click on Overload Properties. This window should appear:
More about this can be found here.
Hope this helps,
Best of luck!
CATIA V5R19 – user & trainer
ANSYS – beginner
RE: Catia V5 Drafting Mode
Was the drawing loaded in the session during the recreation and deletion of the scenes?
To modify the scenes and rename them, the drawing should not be loaded. Sorry that wasn't mentioned in the original statement.
RE: Catia V5 Drafting Mode
I have found answers to some to some of the questions that have come up in this thread.
First:
What is the differance between a partial and a full scene?
If partial is chosen, whatever you do in the scene happens to the model and whatever is done to the model is done to the scene.
If full is chosen, it creates a seperate model withen the model that can be manipulated without changing the main model. It is possible to add parts to a full scene using the following steps.
Place the part you want added to the scene in the main model. copy and paste special into the scene. this will add two of the same item to the tree. one in the main model and one in the scene. It is possible to remove one of the parts from the tree without affecting the anything.
Second:
If views are taken off of a full scene that is not correct, how can you fix it without recreating the views?
A new scene can be made and the drawing view can be linked to the new scene. This updates the view with any labels and text so that you don't have to waste time retyping all of that information.
Hope that helps and provides some clairity.