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transparency in drawing

MaikTheBike
15-Moonstone

transparency in drawing

Hi,

 

can somebody tell me the correct way to show one or more parts of an assembly as transparent in a drawing ?

 

In the assembly I clicked on "Model Display > Component Display Style > Transparent" and the selected component is displayed transparent. So far so good.

Then I saved the style in the view-manager and created a new combined state that includes the new style with the transparent component.

 

Then I created a new drawing and chose the combined state I created. But it doesn't work. The part isn't displayed transparent in the drawing-view.

 

what am I doing wrong ?

 

Thanks,

Maik

 

9 REPLIES 9
kdirth
20-Turquoise
(To:MaikTheBike)

I have always used component display in the drawing.

 

Select Component Display / Style, select component/assembly, select OK, select PhantomTrnsp, and select done.


There is always more to learn in Creo.


@MaikTheBike wrote:

Hi,

 

can somebody tell me the correct way to show one or more parts of an assembly as transparent in a drawing ?

 

In the assembly I clicked on "Model Display > Component Display Style > Transparent" and the selected component is displayed transparent. So far so good.

Then I saved the style in the view-manager and created a new combined state that includes the new style with the transparent component.

 

Then I created a new drawing and chose the combined state I created. But it doesn't work. The part isn't displayed transparent in the drawing-view.

 

what am I doing wrong ?

 

Thanks,

Maik

 


Hi,

I found https://community.ptc.com/t5/Detailing-MBD-MBE/Creating-Drawing-View-with-Transparent-Components/td-p/57210 discussion.

I created two cubes in Creo 6.0.4.0 (1st one with default color, 2nd one with transparent color). Then I placed a view into new drawing, below you can see the result.

transparency.png

Note: I did not test Combined view functionality in drawing view.


Martin Hanák

 States placed on drawings don't include Style or Appearance states, because these cannot be used in drawings, for inexplicable reasons. Style and Appearance states is only useable in the model.

Thanks for your replies.

 

I tried to use the Component Display / Style-Option, but it doesn't seem to work.

 

When I click on Display -> Style-> (select part)->ok then the style menu appears.

I click on phanton-transparent -> done, but the component doesn't appear transparent. I tried it many times, but nothing happens.

 

Martin, your way works, but isn't the part transparent in the model then ?

I only want the part be transparent in some drawing views to be able to see, whats behind the parts.

In the 3d-model the part shouldn't look transparent.

 

Thanks,

Maik

 


@MaikTheBike wrote:

Thanks for your replies.

 

I tried to use the Component Display / Style-Option, but it doesn't seem to work.

 

When I click on Display -> Style-> (select part)->ok then the style menu appears.

I click on phanton-transparent -> done, but the component doesn't appear transparent. I tried it many times, but nothing happens.

 

Martin, your way works, but isn't the part transparent in the model then ?

I only want the part be transparent in some drawing views to be able to see, whats behind the parts.

In the 3d-model the part shouldn't look transparent.

 

Thanks,

Maik

 


Hi,

YES part is transparent in all modes / all views. I'm afraid that functionality you need is not implemented.


Martin Hanák
kdirth
20-Turquoise
(To:MaikTheBike)

Component display does not work in a shaded view.

 

I have tried to use a combined state to create what you are looking for but the style state with transparency does not show on the drawing view.


There is always more to learn in Creo.

It's weird that this functionality isn't implemented. It should be a simple thing to allow you to set Style or Appearance State in your drawing view, just like you select a Simplified Rep or Explode State. But no can do.

 

Ideas for workarounds:

  • Make the component transparent in the model, take a screenshot, add it as an image in your drawing. Downside: Won't update, can't add dimensions or BOM balloons.
  • Make the Default Appearance State transparent (that's the state used in drawings) and then work with the Master State when working with the model.
  • Make a version of your part which is transparent, using family table, merge, copy geometry etc., then use Simplified Reps or layers to manage the display of it. Or even use an Interchange Assembly.
  • Make a Shrinkwrap feature copying all the surfaces of the part, paint it with a transparent color, then use layers to hide it in the model but show it in the drawing.
StephenW
23-Emerald II
(To:MaikTheBike)

Component Display - Style changes the selected component to phantom lines and then depending on whether you choose phantom opaque or phantom transaparent will determine how the components look behind the part.

Opaque will maintian you current hidden lines setting  (no hidden or hidden lines) 

Transparent will allow all part edges behind the phantom part to be displayed as if the part wasn't there but you still have the phantom lines of the original part

iso view with no hidden lines:

StephenWilliams_0-1584455029561.png

 

Iso view with top part set to phantom transparent

StephenWilliams_1-1584455079945.png

 

 

 

Patriot_1776
22-Sapphire II
(To:Pettersson)

I noticed this too.  I was stoked at the ability to create them in the assy, specifically for use in dwgs...only to be bitterly disappointed.  But hey, instead of increased functionality we got a LESS functional but fancier ribbon, WooHoo!  *facepalm*

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