Assembly drawing with external componet context

[MG_10170125]

Hello,
I need to develop assembly drawing of mounting of several brackets on the frame (green lines on the screenshot).
But the frame should not be a component of this assembly. It should only be an external context.
- The mass of the frame should be excluded in the mass property calculate;
- The frame should not be included in assebly BOM;
- The frame should be shown by a thin line in the assembly drawing.
- Frame is a real assembly which I use in another product. And I need the real frame to be associative with the simplified frame-context.
Regards,Max

[tbraxton]

If you are using Creo 7+ you have the option to import the frame into a part and define the geometry as a construction body in the Creo part. This will exclude the frame from mass properties. Construction bodies are also excluded from repeat regions (BOM table). You will be able to include this body in an assembly and constrain your brackets to it as shown in your picture.

To control the display of the frame lines in a drawing of the frame you may have to resort to pen table assignment when plotting.

[MG_10170125]

Thank you!

Unfortunatelly I use Creo 6. Also I have Advanced Assebly Extension and Windchill.

[tbraxton]

For your scenario I would do the following:

Create a skeleton model that will contain the geometry of the frame. This skeleton will reside in an assembly that represents the picture you posted.

Open the skeleton model and import the frame geometry as surfaces, not solid. This will exclude it from mass props but it will be visible.

Add the brackets to the assembly constrained to the frame as needed

Skeleton models do not show up in the BOM unless you specifically include them. They do not contribute to mass or surface properties. They can be displayed in drawing views and can be included during the creation and manipulation of simplified representations and external shrinkwrap features.

[MG_10170125]

"To control the display of the frame lines in a drawing of the frame you may have to resort to pen table assignment when plotting."

Could you please explain how to do it?

[kdirth]

I have always used Component Display to change the reference item to phantom.

Component Display > Style > Select part or assembly in view > PhantomOpque or PhantomTrnsp > Done

[MG_10170125]

Thanks. But I have problem with it.

I'm from Russia and I have to comply with Russian standards of drawing delelopment. In this case it must be thin solid line.

PhantomOpque or PhantomTrnsp - dashed lines and I can't change it https://www.ptc.com/en/support/article/CS175408

[tbraxton]

Before looking into mapping the pens when plotting, try this first.

Modify the Line Style of a Drawing Item

https://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/detail/To_Modify_the_Line_Style_of_a_Drawing_item.html 

[MG_10170125]

I managed to change only one line...

Could you please explain how to change all lines in assemly component?

[tbraxton]

You should be able to select multiple lines to change the font. I have not tested all of the functionality using this approach.

This is an overview of the use of pen tables to control line weights when plotting. You can assign line style by color which will set all lines of a color to a line style when printing.

https://www.ptc.com/en/support/article/CS25880

[BenLoosli]

Bring the frame in as a skeleton model to your assembly.

[MG_10170125]

It can be tested with any sleteton model + shrinkwrap feature. When I paste it in drawing view I can't shown it it thin lines using ''Component Display".

[sacquarone · Accepted solution]

Hello @MG_10170125 

Please let me share what I thins it's the easiest way to configure what you need, if my understanding of your busines need is correct. It consists in:

• Modifying Properties of all the curves in your skeletton
• Changing therefore system color of the entities

=> which will affect later the way how entities will be printed

I illustrate this in little movie (with sound for explanations) attached to this post for guidance in this direction.

Alternatively, as already suggested earlier in this post, you may want to modify your pen table file to drive how some specific system colors (the curves) are affected.

For a guidance in this direction, consider it's a bit harder to do it (if t's the first time you try it), but nevertheless possible according to instructions in article 24802. The suggested technique URL (from this article) should be very useful to understand how this mapping (between system colors in Creo, and way how print entities are produced) is structured.

Regards,

Serge

[MG_10170125]

Hello,

Many thanks for your movie!

Buttom "Properties" (movie timing 1:37) is not active for me. 

I use Creo 6 - is this reason?

Or may "Properties" active in some specific license?

[MG_10170125]

Hello again,

Button "Properties" active only for sketches. 

My frame is not sketch, it's surfaces made by "Shrinkwrap Feature". How to change linestyle for surfaces?