ASSEMBLY AND DRAFTING

[virial]

Hi everydody

I have a big assembbly product and i want to choose which parts of that product can be seen in a isometric view, in drafting workbench.ACtually i take the parts to "no show" in "assembbly workbench" but i think there is an easier way to do it.Is there another way?

Thanks in advance
Javi

 

[tkchiu]

Hi virial,

Some one has already post the reply regarding this topic some time back. I'm too lazy to search that again for you, and so I just write it in here again ...

1) Move your cursor on top of your Isometric View in the
tree (it works equally well for other types of View such
as Section View)
MB3+Isometric view object+Overload Properties
2) The Characteristics Panel comes up
3) Click your Screw/Part which you like NOT to be shown
4) The instance is now displayed on the panel
5) click edit
6) The editor panel comes up
7) And in here you can check/uncheck the followings
cut in section views
Represented with hidden lines
Use when projecting
Shown
click OK after finishing your selection
9) See what you get ...

Hope it helps. Cheers. Kennis Tang.

 

[virial]

Thanks a lot tkchiu , it works perfectly. You have saved me a lot of working time.

Best regards

 

[ogabriel]

The trouble with that methodology is that parts that hide other parts will still hide those parts even if they are deactivated in Overload Properties.
Another way of doing it is to select the ISO view in drafting, in assembly multiselect the parts you want to see in the tree before clicking the graphic to start generating the view. This doesn't work properly when working with TeamPDM (can't say if it works with VPM).
Another way, and probably the best, is to create a Scene of the assembly where only those parts you want to see it visible. Use this scene to create the ISO view you want. This methodology do work with TeamPDM.

Good luck
Ola

 

[tkchiu]

Hi there,
Yes, wholly agree with Ogabriel the view point of that generating the Isometric View from a Scene which pre-defines what parts is showing/not showing is the best way
to manuipulate such situation.

Somehow the Overload Properties method which is aimed to work on Section View is also found to be applicable in here ... could be an alternative to an existing Drawing containing some ISO views ...

"...parts that hide other parts will still hide those parts even if they are deactivated in Overload Properties ..."
Yes, I myself also come across this problem. Seemingly if we
play around those checkboxes, this problem could be gone.

Cheers. Kennis Tang.

 

[goodlook]

Hi everybody,

Can someone explain the functional difference between isolate view and overload properties.

I do have the same question about detailing different components in an assembly. How to detail each and every component of an assembly in draft mode.(most of them in one sheet)?

Thanks

 

[jakey]

Hi goodlook,
In reply to the above questions and yours,

If you isolate a view it will no longer be linked to the 3D model and therefore if the model changes then the view will not be able to be updated to reflect those changes.
You CANNOT re-link the view to the model therefore the view is useless to you.
You use overload properties to hide/no-show individual parts of an assembly or change the linetype of parts in the view (ie dashed, phantom etc).
If you want to detail an assembly and its individual parts on the one sheet, you can use the overload properties in each view to no-show the parts you don't want to see.
Unfortunately when you use the overload properties on a view you can only pick individual parts not products, so if you have a hundred parts to your asembly you have a lot of work selecting 99 parts in each view to no-show.
The best way is to pick the indvidual part you would like to detail from the assembly tree.
This will only create a view showing the part you pick from the tree.
If you hold the CTRL button down on your keyboard and multi-select more than one part in the assembly tree then the view you create will only show the parts you picked not the whole assembly.
So, with the assembly open and your drawing on the screen, tile the window horizontally, Select the create FRONT VIEW icon, in the assembly tree pick the part (or CTRL and multi-select a number of parts) you would like to detail, next select a face to orientate the view, the view appears on your drawing, use the orientation button to position the view to your satisfaction, HEY PRESTO!!!! done.
In addition and in reply to the above messages,
in the overload properties dialogue box, if you uncheck the SHOWN box, the part you selected will not be shown in the view but the view still thinks you want it projected in that view just not shown, so that is why anything behind it will still be hidden by the now NOT SHOwn part.
You should uncheck the USE WHEN PROJECTING icon aswell as the SHOWN icon, then anything behind the part will be regenerated and dispayed properly.
Hope this helps,
Jakey

 

[rpm2]

Excuse my ignorance,

I'm surprised there was no mention of using filters.

Do they not work in v5 ?

Regards,

rpm