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Large drawing: Hatch problem

5 REPLIES 5
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Message 1 of 6
R_Verhees
168 Views, 5 Replies

Large drawing: Hatch problem

We have a rather large assembly of which I'm trying to create a drawing with sectioned views. There is a problem wih the hatch in the sectioned views.

The hatch is not restricted to the parts that have been sectioned, but fills the whole view window.
Also, not all lines seem to be displayed in the view.
This is also the case on a printed sheet, so it's no display error.

Rebuilding the assembly or rebuilding of the views doesn't seem to help.

Mem usage exceeds 1.5 Gb on a P4 @ 3 GHz with 2 Gb RAM and an Nvidia Quadro 750

Is there a solution to this?
5 REPLIES 5
Message 2 of 6
Anonymous
in reply to: R_Verhees

Does the model include elliptical or organically
shaped parts? I just ran into this & ended up hiding the hatch & using
the fill tool on projected geometry.


--
Dave Hoder
Product Design
Engineer
idX Seattle

href="http://www.idxcorporation.com">www.idxcorporation.com
Message 3 of 6
R_Verhees
in reply to: R_Verhees

[quote]
Does the model include elliptical or organically shaped parts?
[/quote]
None, except for the model of a man which I found on one of the inventor sites. But that's hardly an organically shaped part, more a lot of fillet features.

Though I still hope to do it the way it's supposed to work, can you explain some more on how you solved this?
Message 4 of 6
Anonymous
in reply to: R_Verhees


  1. RMB on the hatch & select Hide from the
    menu.

  2. Click on the view to highlight it & select
    Sketch or type S

  3. Click on the Project Geometry button on the panel
    bar

  4. Select all of the lines that make up the border of
    the area you want to hatch

  5. RMB & select Done

  6. Click on the Fill/Hatch Sketch Region button on
    the panel bar

  7. Select your closed loop ( if it's not closed you
    will have to add your own sketch geometry)

  8. Select the Enable Hatch option from the dialog
    & choose your hatch 


--
Dave Hoder
Product Design Engineer
idX Seattle

href="http://www.idxcorporation.com">www.idxcorporation.com
Message 5 of 6
R_Verhees
in reply to: R_Verhees

Dave,

Thanx for your explanation.

For all: i've tried a different approach: use multiple sheets and only one view on each sheet.
This doesn't solve my problem, but might have given away a clue: a section view in one direction is messed up with the hatch filling the whole view, a cross section in the perpendicular direction doesn't have that problem. Strange huh?

Also, i've been talking to the support departement of our local reseller and they suggested the solution described in the knowledge base under nr. TS66809, which is to remove the secion line from the base view, draw another one in sketch mode and offset it a little from the original one. This was originally an ACIS kernel bug, but ACIS is no longer in the picture since release 5.3, isn't it?

This didn't solve my problem however...So if any one has any ideas: they're welcome!
Message 6 of 6
R_Verhees
in reply to: R_Verhees

Solved, finally!

It turned out to be a tiny ball in a ball bearing that appeared to have or show a large rectangular solid (larger then a 3mtr high machine!!) that was not visible in the bearing assembly or aball model itself.


This explaines also why not all modellines were visible: they were hidden by the sectioned non-existant solid....

I downloaded the bearing from a vendor's site and replaced i t with one fom the Inventor library: all's well now!

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