Design in Context

[amnon]

Hey

I use Design in Context (Top Down). Few days ago I made some chcnges in Options,
and now I have a lot of problems . I created Counterbored hole on Part1, than
I created hole on Part2 with constraints-concentricity with Counterbored hole.
Now when I change positon of Part1 it does not affect position of hole on Part2.
What should I set up in Options?

Merry Christmas
Amnon

 

[MrCATIA]

Hey, Merry Christmas and Happy New Year to you!

I'm not sure the TOOLS + OPTIONS change is what caused your link problem. I'd suggest you check the link in the EXTERNAL REFERENCE branch of the PART2 tree, and I'm guessing that you'll probably have to replace the link to the PART1 hole.

If you want to check your TOOLS + OPTIONS, look at the GENERAL options page in INFRASTRUCTURE + PARTS INFRASTRUCTURE. I suggest activating the following two options:
o CONFIRM WHEN CREATING A LINK WITH SELECTED OBJECT, and
o ONLY USE PUBLISHED ELEMENTS FOR EXTERNAL SELECTION KEPING LINK

(but changing these options should not have caused your problem)

 

[amnon]

Thank's

I think it was:
-Keep link with selected object
Allow publication of faces, edges, vertices, and axes extremities

Is it possible to add External References (additional surface) to existing one in Part ? (to place one Part on the other)

Amnon

 

[MrCATIA]

Sure, you can add as many External References as you want

Just remember:

1. Since these are contextual links, you must always work in the same context (same assembly) when you want to add or replace links

2. Links are one direction only - child part to parent parent part. No loops are allowed - you can't make a link from the parent back to the child.

 

[MrCATIA]

more info

I notice that Amnon's thread is very popular and has many viewers. I'm including this link to Amnon's original thread, which includes some more information about Contextural Design and External References.

http://www.3dcadforums.com/cad-communities-7/catia-forum-10/external-references-2106.html

This is a very powerful feature of CATIA V5 when used properly, and good training is key to successful implementation.

 

[amnon]

Hey,

Could You tell me few steps, how can I add External References ?

Amnon

 

[MrCATIA]

(I thought you knew how to do this )

Okay, let's assume you have an assembly open with several parts including Part.1 and Part.2. Part.1 has a surface, and Part.2 has a solid (PartBody) and you want to split the solid with the surface. In other words, you want the surface from Part.1 to be linked as an External Reference in Part.2

Let's also assume you have your Tools+Options set as we mentioned above, and the surface is published in Part.1

Two ways you can copy the surface as an External Reference:

1. The automatic way. With Part.2 as the active part in the assembly, just add the split feature and select the surface in Part.1 This will automatically copy the surface with a contextual link back to Part.1 - the surface is now an External Reference in Part.2

2. The do-it-yourself way. Copy the surface in Part.1 and Paste Special With Link the surface into Part.2. This will make a CCP link, with the pasted surface being an External Reference. Now you can split the solid with the pasted surface.

That's it. If the surface changes in Part.1, the solid in Part.2 will also change.

 

[amnon]

(I thought you knew how to do this )

as you know I am beginner (patience is needed).
I do not know why, ........... but I do not use Publication, and designing in Context works
(I hope so).
Somehow I lost connection Part 1(slider) with Part 2(mandrel). I have been trying to link Part 1 and Part 2 again. As You mentioned below, I copied Surface in Part 2 and pasted it in Part 1 but It does not work. Option Paste with link is not active.
Could You recommend me any book about Design in Context.
Thanks a lot

Amnon

 

[MrCATIA]

Using Publications is not required, as long as your Tools + Options have the ONLY USE PUBLICATIONS option deactivated.

Thanks for including the picture - it helps understand what you're doing.

Now, could you verify something for me. Looking closely at the tree of the assembly of parts, there is a little icon in front of each part and the icon includes 2 little gears and a red axis. Most of the parts probably have blue and yellow gears. What color are the gears in front of the Part.1 (slider) part?

 

[amnon]

Using Publications is not required, as long as your Tools + Options have the ONLY USE PUBLICATIONS option deactivated

Clear,

By the way, could You explain me meaning of all icon colors ?
Thanks

Amnon

 

[MrCATIA]

Amnon, I suspect your problem is due to one of 2 things: either the CATProduct is not the original assembly you used when you first made the External Reference links, or you're trying to add new links to a part instance that is not "in context"

The latest picture you attached shows instances in different contextual states. Thank you for the picture, but you didn't tell me what type of icon your part has?

In my attachment, I've tried to explain what the different icons mean. I hope it's clear.

If what I suspect is correct; activate the contextual instance (green gear) of the slider, and try again to use the surfaces from the mandrel to make your hole. I suspect you may have had an out-of-context (brown gear) instances active, which prevents you from making new External Reference links.

Once you have the green gear part active, also use EDIT + LINKS to check the status of your External References

 

[amnon]

Hey MrCATIA

The latest picture you attached shows instances in different contextual states

is it wrong? Some parts are linked up to assembly by means of constraints (bolts etc.). Is it possible to make all assembly in context?

Thank you for the picture, but you didn't tell me what type of icon your part has?

Attachment

In my attachment, I've tried to explain what the different icons mean. I hope it's clear

image size is too small, I can't see, what did You wrot there.

activate the contextual instance (green gear) of the slider, and try again to use the surfaces from the mandrel to make your hole

Green gear is active. and all external references as well.

In my attachment, I showed problem with joint slider-mandrel (I've lost this contextual joint (surface-surface) and I can't get it back). When I try to conect slider-mandrel by means of Contact Constraint I receive: "Loop design between geometry and constraints"

So my request is ...... If You could take a look at my assembly (entirely)

Amnon

 

[MrCATIA]

Amnon; I think we are talking about different things here. I thought we were talking about External References, but you say in your last post the problem is with Assembly Constraints.

"Design in Context" is designing parts in the context of other parts in an assembly, using links (External References) to share features between parts. It has very little to do with Assemblies and Assembly constraints.

You asked several questions in your last post:

1. From what I can tell, your assembly is not wrong. The different colored icons only indicate the contextual state of each instance.

2. The instance called "Ramie_2.1" has an icon with two gears, blue and green, meaning this instance is the contextual one.

3. I had to reduce my picture to meet the size requirements for attachments. How did you attach your bigger picture? Try to copy my small attachment to another program (like PowerPoint) so you can resize it bigger.

4. The Loop error message is correct. Since you already have external references into "Ramie_2.1" adding assembly constraints between the two parts will create a loop. The only Assembly constraint you need on the green gear part is a FIX. "Ramie_2.1" should be in the correct position if it is "designed in context." You will only need to add Assembly Contraints to the other instances of the slider (Ramie_2, Ramie_2.2, etc.)

I hope everything makes sense.

I'm trying to help you here, but you really should try to find a local instructor who can teach you what "design in context" is all about.

 

[MrCATIA]

Ferdo posted the following link in the CATIA Forum on Eng-Tips.

Since this thread has had such a high number of reads, I wanted to share this information on Links and Design in Context for everyone to read. This is Part 2 of a 5-part article that appeared in the CATIA Operators Exchange (COE) newsletter back in 2005.

COE

The author is Julie Cyrenne from Dassault. She is one the smartest CATIA users I have ever met, she's a great teacher, and she really helped me alot when we worked together at Boeing.