Hide tangent line & convert centerlines

[sundeep198]

Hi all,
I deal with creation of tube / pipe drawings in Catia V5 R18 & 19 from models.
My major time is spend in hiding the tangent lines & converting the center-lines. The drawings are big in size. Refer the attached image file, this is just a view of a drawing.

http://files.engineering.com/getfil...73d-a83e-269375e52067&file=CATIA_TUBE_DRG.JPG

Is there a setting or macro which can help me.

Regards,
Sundeep

 

[GELFS]

Hello Sundeep,
You may try the following
[ol 1]
[li]Select all views[/li]
[li][Properties]>[View Tab]>[clear Fillets checkbox]>[Apply]>[OK][/li]
[/ol]
Tangent(boundary) lines shall disappear

-GEL
Imposible is nothing.

 

[sundeep198]

Thanks GEL this works fine.
Any idea about the centerlines.
regards,
sundeep

 

[GELFS]

You are welcome.

Any idea about the centerlines.

As far as concerning the centerlines I need to know how these have been created.

-GEL
Imposible is nothing.

 

[ferdo]

Hi,
Better upload a sample view in a model file (when you said model, I suppose is a v4 file). Sorry, I'm not able to download your picture...

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

https://picasaweb.google.com/103462806772634246699/

 

[itsmyjob]

For the center line you can use Generative view style (check documentation) so wireframe will inherit line type.
You will have to keep the center line in show in 3D.

Eric N.
indocti discant et ament meminisse periti ​

 

[sundeep198]

The centerlines are derived from 3D.
CatiaV5 R18 & R19

 

[GELFS]

Hello Sundeep198

You may try the following:

[ol 1]
[li]Select all views in the drawing[/li]
[li]Select [Properties]>[View Tab][/li]
[li]Clear [Fillets] checkbox[/li]
[li]Check [Hidden lines] checkbox[/li]
[li]Check [3D Wireframe] checkbox and make sure that the [Can be hidden] radio button is pressed[/li]
[li]Select [Apply]>[OK][/li]
[/ol]
Note: All these setting can be done in the [Tools]>[Options]>[Mechanical Design]>[Drafting] if you need to have them as standard settings


-GEL
Imposible is nothing.

 

[sundeep198]

Hi GEL,
I am getting what i need, but hidden lines are not required.

 

[GELFS]

Hi Sundeep198,
This means that
[ul]
[li]The centerlines in the relevant catpart already have the dash-dot linetype.[/li]
[li]The used GenerativeView file has been set so that for the wireframe elements in the drawing inherit their linetype from the model[/li]
[/ul]

Yes, all required settings can be done by creating a new or modify an existing Generative View file.

-GEL
Imposible is nothing.

 

[Gilgamesh99]

Im having the same issue. How can the centerline be shown with enabling the hidden lines?

 

[GELFS]

How can the centerline be shown with enabling the hidden lines?

I'm not really understand your question. Can you explain a little bit more?

-GEL
Imposible is nothing.

 

[Gilgamesh99]

What I mean is how can the axis (usually created with a polyline for this kind of tubes) be shown as centerline and, at the same time, not to show the hidden lines? Just as sundeep198 is showing in his image in the first post. What could be the best way to achieve it?

 

[GELFS]

Hello Gilgamesh99

A Drawing is composed out of Views. Each View is generated by a View Generator Machine. This machine has a number of parameters(properties).
A small part of these parameters is shown in the Properties dialog box in its View tab. In [Properties]>[View] are appearing, let's say, only the 'main switches' but not all the parameters.
For example, if we want to show in a view the wireframe features of our model we just need to check the [3D Wireframe] option. This main switch will allow us to turn on/off the wireframe features but will not allow us to specify how this features will be presented in the view ie we cannot define the 3D Inheritance parameters of a Wireframe feature like the Linetype one, which controls whether the feature in the drawing view will inherits its linetype from the model.
All these parameters are defined in a Generative Style file (which is an Xml file) which is read by CATIA.
Now that we have basic understanding of how CATIA works, lets move on how to access and edit these parameters.
We have two ways to go. One, to directly access the Generative Style file(s) folder and edit the relevant file with an XMLEditor (or any Text Editor like Notepad). Two, to do the work through CATIA. The full set of parameters is in the [Properties]>[Standard tab] if you click [More...] button but are not editable unless you are in Admin Mode. So, in this case we need to run CATIA in Administrator Mode, which is another story.
In the first case, just we need to:
[ul]
[li]Get in the C:\Program Files\Dassault Systemes\B20\intel_a\resources\standard\generativeparameters directory (Your directory may be different)[/li]
[li]Make a copy of the file DefaultGenerativeStyle.xml and rename it to what you like.[/li]
[li]Open the file and locate the Node 3D Inheritance. It will look like this:[/li]

- <std:node name="3DInheritance">
  - <std:node name="Wireframe">
  - <std:node name="Color">     <std:enumval name="YesNo">No</std:enumval>  </std:node>
  [b]- <std:node name="Linetype">  <std:enumval name="YesNo">[u]No[/u]</std:enumval>  </std:node>[/b] 
  - <std:node name="Thickness"> <std:enumval name="YesNo">No</std:enumval>  </std:node>[/li]
....

[li]In the line where the value of LineType property is defined (the bold one) change the underlined value to Yes[/li]

- <std:node name="3DInheritance">
- <std:node name="Wireframe">
  - <std:node name="Color">     <std:enumval name="YesNo">No</std:enumval>  </std:node>
  [b]- <std:node name="Linetype">  <std:enumval name="YesNo">[u]Yes[/u]</std:enumval> </std:node>[/b]
  - <std:node name="Thickness"> <std:enumval name="YesNo">No</std:enumval>  </std:node>
....

Now that we have completed the customization of our new Generative View Style file let's implement it[/li]
[li]Go back to your drawing and open the properties dialog box of a view. At lower part of view tab, open the [Generative View Style] combobox and select our customized new Generative View Style file.[/li]
[li]All visible wireframe features in the model will be presented in the drawing view with the same linetype as in the model.[/li]
[/ul]

-GEL
Imposible is nothing.

 

[sundeep198]

Hi GEL,
I modified the .xml file, but i am not able to trace Generative View Style from file view properties.
Attached is what i am able to see.

http://files.engineering.com/getfil...6b7b&file=properties_dialog_box_of_a_view.JPG

Regards,
Sundeep P.

 

[GELFS]

Hi Sundeep,
Use the vertical slidebar to move down and you will see the rest of the tab fields.

-GEL
Imposible is nothing.

 

[Gilgamesh99]

GELFS:

I tried the above method on CATIA V5R16 and there was no Generative View Style menu at the bottom of the view tab. On the other hand, using CATIA V5R20 there it was, unfortunately (even after the xml archive modification) it was dimmed and unable to activate. Any ideas what the problem could be.

Thanks in advance for your great help!!!

 

[GELFS]

Hi Gilgamesh99.

Two things may happen:
One, you have selected more than one view before opening of the |Properties| dialog box. Try again with only one selected view. For some reason the [Generative View Style] combo box is disabled in case of multiply views selection.
Two, Your system administrator has locked this option. Contact your system administrator.

Note: In case we like a post then we shall star it. By this, other viewers are also informed about interesting posts.

-GEL
Imposible is nothing.

 

[GELFS]

One more thing may be the root of your problem. That the Generative View Style functionalities are deactivated.
Go to [Tools] > [Options] > [Mechanical Design] > [Drafting] > [Administration] tab, and clear the [Prevent generative view style usage] check box. This activates the generative view style functionalities.

-GEL
Imposible is nothing.

 

[Gilgamesh99]

Thanks a lot. As usual you're a great help