Clear parts in assembly drawings 1

[dhinners]

I would like some forum feedback on how people deal with clear parts in their assembly drawings. For example, if you have a plexiglass guard that you want show the edges of, but also show the items behind it. My best solution so far is to make a configurations in the assembly with the guard hidden / not hidden. Then I insert my drawing view using the hidden configuration, and show the guard using the Alternate Position View. The only drawback is the part comes in in phantom line font.

Any thoughts?

 

[DetroitPickles]

Man. Don't you hate it when folks ask questions like this? I have a bunch of steel and stainless parts. I don't have any clear parts. Now, I have to go and make a clear one, just so I can learn something like what you are talking about.

Learning new things ought to be outlawed. Old men like me shouldn't be learning new things, or is that old dogs?

Mr. Pickles

 

[testy]

I am not sure if this is what you are after, but have you tried setting the plexiglass transparency to full. You will find this option under Document Properties-Colors-Shaded-Advanced.

HTH

Ray

 

[SBaugh]

Why can't you just use Hidden lines Visible? That will show the edges of the clear Guide and also the items underneath. Except they will be in hidden line format. Which is accurate...because its underneath the guide.

Also check your Line font in tools\options\document properties\line font There you can change your Line font's according to what your needing.

Best Regards, Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.3dmca.com

faq731-376
When in doubt, always check the help

 

[TheTick]

You can change the line font of your alternate position view. In the feature manager design tree, expand the alternate view so that you can see the icon for the assembly. Right-click on the assembly, and select "Component line font". Here, you can choose a specific line font. Be careful to make sure that you select "from selection" and not "all views"

With "component line font", you can also color the line by specifying a layer. Gravity is a harsh mistress.

 

[drawoh]

dhinners,

Drafting rules do not make distinctions between transparent parts and non-transparent parts. If something is behind a part you know to be transparent, you should use hidden lines.

If you are really determined to do this, you can attach phantom lines to the ouline of the transparent part, then hide the transparent part.

JHG

 

[dhinners]

I agree that drafting rules dictate that any items behind transparent parts should be shown as hidden. However, if you turn on hidden lines, you will see all edges of all parts throughout the assembly.

The main area where this becomes an issue is for technical manuals, where the drawing you create does not typically follow strict drafting standards. Also, your views are often isometric which really looks messy in hidden line mode.

If you can reuse your assembly drawing for an illustration in a manual, you have saved time & increased your productivity. The issue is generally that a drawing is not necessarily the same thing as an illustration.

I have used the method of converting edges of a part, then hiding it in the past. The main drawback there is if you want to attach associative balloons.

Changing the component line font works well. Why didn't I think of that? Oh well, I have to keep learning, if only to keep ahead of the forgetting.

 

[MadMango]

For technical manuals, have you tried shaded views? SOmetimes for complicated parts or assembly drawings, I'll plop in a shaded isometric view. The guys on the assembly line seem to like them alot, even if they only see them in gray scale. Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."