I have a question concerning how to optimize model creation to maximize downsizing of model size.
I have designed bumper to a car, which at the end has 700mb. It is really huge, and because of that model works really slow. Are there any possibilities to optimize it? Maybe there are come features which consume more computere permofmance than others, for example instead of doing blends sepateretely I should do them in one step, or instead of doing 'unite with defining regions' I should first trim the parts which will be removed and then do the clear unite?
Do you know some nice moves?
There are some very heavy features and these can be replaced by others much lighter IMO.
I attach you two files with the same geometry, one wheigs 3Mb, the other wheigs 4Kb (NX11).
Pattern Features vs Pattern Faces where possible.
Another reason that makes files heavy is to use too narrow modeling tolerance where it is not necessary.
Following are the best Practices
Load option: Use "Partial Loading" it shows enough information to show the part.Making the part the work or displayed part causes NX to fully Load the Part.
Reference Set: use Reference sets to Display only the needed geometry.
Load Only Need Components: Large assembly you may want to load no components and only turn on the necessary components as needed.For companies that deal with large assembly and open them a lot it is more efficient to use " Design in context" , This Design in context is TC application.
Filters/set: when working on specific assembly for an extended period of time create a components Filter so that you can Quickly Return to the previous configuration.
Use faceted bodies consist of the outer skin of the body and approximations of the solid body.
Make a component the work part, the system "grays -out'' the non-work parts.Set Preferences >Assemblies >
Emphasize because of this work part remains displayed in its current colour, other assembly in dimmed in colour.
Make Back Face culling enabled it will reduce rendering.
Set Frame Rate fix in visual perference.
Its difficult to guide you without seeing the actual part but bleow are some of my to reccomendations that are valid in the majotity of the cases when it comes to large parts sizewise.
That really sounds like quite a model there.
I hope this will help you somewhat
With all the previous comments from other users,following are some suggestions that you can use in combination to reduce the part file size.
Save Options: As mentioned earlier Toggle on ‘Compress Part on Save’.
Toggle off ‘Save Data for Fast Rollback and Edit’. This option is stored with part and can be set in ‘Customer Defaults’. Toggling off this option will reduce the file size.
Part Cleanup: The very first command that I will use to clean/delete the unused objects from the part file. Use actions, Simple Cleanup, Moderate Cleanup, Moderate Delete. Depending upon the how you have constructed the model, use Serious Delete Actions options carefully.
Preview: File > Properties > Preview tab
Toggle off Store Preview (Part Preview) and Store Previews (Model View Preview).
Toggling off Model View Preview will reduce part file size to some amount (which can be ignored).
Heal Geometry: File > Export> Heal Geometry.
As Heal Geometry uses tiny tolerance, exporting part with this option will reduce part size considerably. At the end of the operation, Heal Geometry Statistics will be displayed.
From documentation “The Heal Geometry command exports the work part to another NX part to perform any required healing operations on the selected solid entities. As a result, after healing completes the work part is the same as before the application starts.” Refer the documentation link for more information. Heal Geometry.
When the 'Heal Geometry' command is used there is an internal step which seeks to remove any duplicate curves and surfaces. Duplicate curves or surfaces are of the same class and are spatially and parametrically coincident. It reduces the size of a part by sharing geometry.
The major contributor to the file’s size is the feature data. This feature data is saved to retain the all parameterizations for editing each feature. You can also consider the following options if parametric feature data is not the main concern.
Optimize Face: 'Optimize Face' command can also be used to reduce the file size, but it will produce dumb bodies.
Parasolid: Export as Parasolid and import back in NX,save. As it will have only dumb bodies, Synchronous modeling can be used to edit the model. Editing will be depend upon the complexity of model and changes required.
Maybe there are come features which consume more computere permofmance than others, for example instead of doing blends sepateretely I should do them in one step, or instead of doing 'unite with defining regions' I should first trim the parts which will be removed and then do the clear unite?
Rather than applying blend/chamfer to the individual instance of pattern feature. You can enable "Blend All Instances" and "Chamfer All Instances" by defining the system environment variables "NX_ENABLE_BLEND_APPLY_ALL_INSTANCES", "NX_ENABLE_CHAMFER_APPLY_ALL_INSTANCES" respectively, with value 1. With this you can apply blend/chamfer to the faces of pattern feature at once. Unfortunately, it does not work for Pattern Face.
Another option to the "export Parasolid -> import" process is to just remove parameters (resulting in a dumb solid)
Menu -> Edit -> Feature -> Remove Parameters
But note - you DO lose ALL feature data, so any subsequent edits must be done via Synchronous modeling.
Also, I don't know if they result in exactly the same size, or if one method is consistantly smaller than the other (by a meaningful amount)
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled