CC Components missing in idw drawing in large assembly

[mdahl74]

Having trouble with placing a larger Assembly into a IDW drawing .

When i place the Assembly into the drawing some of the CC parts are missing? , I have 6 stantions in the sub assembly of a hopper and when i look at the IAM every thing is present and correct but as soon as i place it into the IDW i am missing 2 of them ?? if i look thru the browser they are in the tree and visible .

there are other non CC parts missing also like sheetmetal parts etc as well as other.

If i create a drawing with just the hopper assembly it comes out perfect ?

using version 2019

Gaps in rail , top cover missing and tread plate sheetmetal gone

[Xun.Zhang]

Hello @mdahl74,

How about create a new level of detail and only leave these two components unsuppressed and than create new drawing view to see if it works or not.

another one is, edit the view, switch the design view to Master.

Please let me know your result then.

[mdahl74]

I have tried different LOD's and also tried different view and changing to master etc , even made the couple of handrails "custom" parts and stored with in project file just to rule out CC issue , as you might be able to see from the pictures even the Motor has only the motor cover , just seems really random

I am able to view the hopper correctly and create drawing of it but once it becomes a sub-assembly of the whole project it is having the issue .

The Building behind which the hopper is located is generated from a 3d scan that has been modeled out and is full of Part files could this cause the issue ? total part around 400 pieces .

[mdahl74]

no luck solving this one .. the only work around i thought was working was to

1. make the entire assembly a simple part

2. make the drawing from the simple part and make the views

3. then the wheels fell off again when making a pdf for a presentation the colours assigned to the new work were missing !! all mono tones

the only work around after many painful hrs i ended up exporting the idw to a inventor dwg file , then opening the dwg in auto cad  and then finally printing with an output for pdf  

[johnsonshiue]

Hi! The behavior is certainly wrong. Four possibilities. 1) The CC components are Reference Component and they are not shown in the view based on view setting (edit the view -> Displace Options -> Reference data). 2) The parts have bad bodies. They are not shown correctly. 3) The components have interferences. Check Inspect -> Interference Analysis. Clear out the interference. They can cause design issues. 4) The parts are excluded incorrectly, because Inventor thinks they are behind some components, which is false.

Please share the files here or send them to me (johnson.shiue@autodesk.com). I would like to take a look at it and understand the behavior better.

Many thanks!

[mdahl74]

Johnson , I have just sent you an email and will grant you access to the files

[johnsonshiue · Accepted solution]

Hi Michael,

Like I replied in the email, the issue seems to be related to geometry placed in extremely outside of valid model range. Inventor has a fixed valid model range (+-100m in X, Y, and Z) and each piece of geometry should be less than 100m long. For more detail, check the following page.

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2017/ENU/Inventor-Help/files/G...

Regarding moving the geometry back to origin, here is the procedure.

1) Open the part with out of bound geometry.

2) Create a UCS based on the geometry.

3) Place the part or the assembly to a new assembly.

4) In the new assembly, create an assembly UCS at origin (0, 0, 0).

5) Create Constraint -> Constraint set -> pick the UCS in the part and pick the UCS in the assembly.

Now the geometry should be back to the origin.

Many thanks!

[lena.talkhina]

Hello @mdahl74  !

Great to see you here on Inventor Forum.

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