NX X How do you fix missing visible edges in assembly drawing views or creating section view.
2021-10-06T23:27:12Z
NX for Design
Summary
Details
If you are unable to create section view or experience missing edges in a drafting view, either silhouettes, smooth edges, or visible edges, how do you fix this problem? The problem could happen to any part that has self-intersection geometry, which is found by Examine Geometry.
1. If the part was created in NX, then you would need to focus on fixing the features that cause the self-intersection geometry or other failures reported from the Highlight Results of Examine Geometry.
2. If the part is an un-parameterized body, then you can use Optimize Face, (since this operation would remove parameters from the part).
Go to Modeling and locate the component whose edges are not visible in
your assembly drawing and set it as Work Part and Displayed Part.
a) In Modeling go to menu Insert -> Synchronous Modeling -> Optimize ->
Optimize Face
b) Select all the entities by Ctrl A.
c) OK -> you should see this dialog:
-> Click Yes to Optimize the Faces and correct the geometry.
d) Go To Drafting and create base view or section view or update existing
views.
3) Heal Geometry:
a) Go to Modeling and locate the component whose edges are not visible in
Assembly and set it as Work Part and Displayed Part.
b) Go To Menu File -> Export -> Heal Geometry. Perform Heal Geometry
operation and save the healed Part. Please ensure the model geometry has
not been changed.
c) Make parent assembly as Work Part and Displayed Part.
d) Go to Assembly Navigator and use Replace Component Tool to replace
original component with Healed Component.
OS: n/a
OS Version: n/a
Product: NX
Application: DRAFTING
Version: V1847
Function: DRAWING/VIEW
Ref: 002-7005203
Solution
If the part fails Examine Geometry with Self-Intersection geometry, Tiny and Misaligned objects, Spikes/Cuts, Consistency and Face Intersections, there are several workarounds that you can try:1. If the part was created in NX, then you would need to focus on fixing the features that cause the self-intersection geometry or other failures reported from the Highlight Results of Examine Geometry.
2. If the part is an un-parameterized body, then you can use Optimize Face, (since this operation would remove parameters from the part).
Go to Modeling and locate the component whose edges are not visible in
your assembly drawing and set it as Work Part and Displayed Part.
a) In Modeling go to menu Insert -> Synchronous Modeling -> Optimize ->
Optimize Face
b) Select all the entities by Ctrl A.
c) OK -> you should see this dialog:
-> Click Yes to Optimize the Faces and correct the geometry. d) Go To Drafting and create base view or section view or update existing
views.
3) Heal Geometry:
a) Go to Modeling and locate the component whose edges are not visible in
Assembly and set it as Work Part and Displayed Part.
b) Go To Menu File -> Export -> Heal Geometry. Perform Heal Geometry
operation and save the healed Part. Please ensure the model geometry has
not been changed.
c) Make parent assembly as Work Part and Displayed Part.
d) Go to Assembly Navigator and use Replace Component Tool to replace
original component with Healed Component.
Notes and References
Hardware/Software Configuration
Platform: allOS: n/a
OS Version: n/a
Product: NX
Application: DRAFTING
Version: V1847
Function: DRAWING/VIEW
Ref: 002-7005203