Transparent part in draft?

I have a test fixture to hold a water tank during pressure test, I wish the
tank to be reference only. I have switched the tank to be outlined as
phantom but how do I make it totally transparent so that the jig outline,
behind the tank, shows up as solid lines and not hidden detail?
Reply to
Phil Evans
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Not possible that I know of. If you find an answer be sure to post it here because I've been looking for that one too.
Another possibilty would be to make the view Shaded instead of Wireframe (or add an additional view for this). Next, in the assembly file make your tank transparent. Now back to the drawing file, your shaded view should have updated accordingly. Also, make sure you set your transparency in the same configuration as your drawing view (in SW2004 the component transparency is configuration dependent, but I can't remember how earlier versions handled this).
And another possibily that's only good if you have a color plotter is to separate all your parts onto separate layers with different colors (in the drawing file). It won't make the lines solid, but will assign the different colors to them. There's a sample macro in the SW2004 help to create the layers as well as a macro called layout.swp at:
formatting link
can't remember if either one of those did the colors or not tho, but it's a start. There's also layer options for lineweight, but I've never experimented with that.
Good luck with your search, Ken
Reply to
TinMan
I was thinking about a macro that would create a 3D sketch by "convert entity" ing all the edges in a part. You could then hide all 3d and show only the sketch in 3D and in drawings Would it fit your needs ?
Thanks for the link, TinMan. Actually, Layout is not free any more. It is now a part of the "SolidPlus macros" pack sold for $99
formatting link
Layout creates a layer for each part and assings it the part's color, or a random one.
Reply to
Philippe Guglielmetti
If your test fixture and tank have been modelled as separate parts in an assembly, you can insert each part into the drawing independantly. Then you can align them horizontally and vertically by origin assuming the origins are in the right places.
If the items are separate bodies in a multibody part file, you can make two configurations, each with one of the solid bodies deleted. Then insert the part into the drawing twice, once for each configuration and align as before. At least your origins will be in the right place this time!
Hope this helps a bit.
Ralph
Reply to
Ralph
Perhaps something can be worked out wit halternate position views? I don't use them often enough to be sure it would work.
Reply to
Dale Dunn
If the geometry of the tank is simple enough, there is one possibility that will work well but it will require a little bit of work.
Convert all of the visible edges of the tank in the drawing by either selecting individual edges or entire faces and clicking convert entity. Then right click on the tank and Hide Component. Then, select all of the converted geometry (window select is fastest) and adjust the line font to whatever you want.
Hope this helps.
Reply to
Seth Renigar
You would have to have a configuration in your assembly that has only the tank showing in it by hiding all the other parts then use the alt position view and use the tank only configuration for the alt position view. It will then show the tank in phantom and everything below it will show up as if it wasn't there.
Reply to
J
As others in the thread have mentioned...
Use an Alternate Position View.
I have done this in the past and it works very well.
Reply to
Arlin
Awsome solution guys! I just tried it and WOW no more converting edges. The cool thing is how easy it is to change the phantom part or have many phantom parts! Tons of possibilities! Who thought of this?!?!?! My appreciation! Once again this group has paid for itself!
> You would have to have a configuration in your assembly that has only the > tank showing in it by hiding all the other parts then use the alt position > view and use the tank only configuration for the alt position view. It will > then show the tank in phantom and everything below it will show up as if it > wasn't there.
> > I have a test fixture to hold a water tank during pressure test, I wish > the > > tank to be reference only. I have switched the tank to be outlined as > > phantom but how do I make it totally transparent so that the jig outline, > > behind the tank, shows up as solid lines and not hidden detail? > > > > > > > > >
Reply to
3d
Thank you, that worked great.
> You would have to have a configuration in your assembly that has only the > tank showing in it by hiding all the other parts then use the alt position > view and use the tank only configuration for the alt position view. It will > then show the tank in phantom and everything below it will show up as if it > wasn't there.
> > I have a test fixture to hold a water tank during pressure test, I wish > the > > tank to be reference only. I have switched the tank to be outlined as > > phantom but how do I make it totally transparent so that the jig outline, > > behind the tank, shows up as solid lines and not hidden detail? > > > > > > > > >
Reply to
Phil Evans
Reading this message gave valuable clues, but I find that the constant use of the word "it" can leave a user who is not a conversant with the situation to wonder just what "it" refers to. This is an all to common problem in technical manual writing, so it is not unusual.
"It" can be INCREDIBLY confusing.
Bo
Reply to
Bo Clawson
Hey BO,
Who the hell made you God of IT. 3d GOT the solution to the problem he had. Seems like he got IT.
Bo Claws>
Reply to
J
The intent of this groupd with a public forum is that the information will be usable for a wide range of users so all who are interested can benefit without each user asking the same question over and over again.
When you use a reply on a subject to explain it then explain how it might work if they are put together to restrain it, well...
I can not imagine what the real meaning is from such a sentence, and neither can most users of this group.
I respectfully submit that clarity counts.
Bo
Reply to
Bo Clawson
Bo,
Don't ya think that's being a bit anal ??
Most folks read through the thread, not just an arbitrary reply. I don't think many will have a problem understanding the problem, or the solution.
Regards
Mark
Reply to
MM
Maybe that's his problem. There's no sun shining where he's at and he cant see thru the sh it
MM wrote:
Reply to
J

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