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Downsizing of model size

Experimenter
Experimenter

Hi all,

 

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?Cat Very Happy

9 REPLIES

Re: Downsizing of model size

Siemens Phenom Siemens Phenom
Siemens Phenom

Do you have 'Compress Part on Save' toggled on under customer defaults?

File  > Save > Save Options > Compress Part on Save.

 

Re: Downsizing of model size

Experimenter
Experimenter

Yes, it is toggled on. What about different ways to achieve the same effect, are there different approaches in which some are faster than the other?

Re: Downsizing of model size

Phenom
Phenom

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.

 

 

Re: Downsizing of model size

Valued Contributor
Valued Contributor
Hi goral,
if you want light and quick editable Part you need right part construction with wide tree(unions and substracts on end of construct) and easy connections of features.
Blending of radiuses is better implemented to each subparts of part construct.

If you want smaller part dont make Wave Links from whole parts. Use only faces which you realy will need.

Faces which are produced from Blend function make part also bigger.
Some times you can make a compare with size of clear parasolid(X_T format) then you can find out how arduous ist your constrution.

Best Regards
GL

Re: Downsizing of model size

Genius
Genius

Hi Goral,

 

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.

 

 

RRG

Re: Downsizing of model size

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Goral,

 

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.

  • First major issue that resides in majority of parts that I have come across over the years is that enginners tend to copy reference geometry into the actual design part. I do reccomend to check for and eliminate (delete) referense data out of the part. If reference data is needed put it in a separate reference part and use the assembly function to reference.
  • Im kind of suspecting that you are using Extract Geometry quite heavily. I would primarily reccomend to try to keep your extracts to a minimum. In the majority of the large parts I have encountered over the years this is another of the most frequent issue identified. In most cases the extraxt are not really nessceary. Concider your modeling thechniques.
  • Should you use lots of Extracted bodies with the same time stamp make sure you extract the original body for oll of them and do not do extract on extract (otherwise you will not benefit form the last bullet in this list)
  • Turn on Share Geometry on Save

 

I hope this will help you somewhat

 

Best Regards

Fred

Re: Downsizing of model size

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @goral,

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. 

 

  • Delete the faceted representation if present in the work part. Menu> Assemblies > Advanced > Representations > Delete
  • There will be copies of the tool bodies in the part file for the Boolean features such as subtract. When the target body feature is edited there is no need to update tool feature. It is possible to reduce the file’s size by using the Boolean option in the Extrude/Revolve feature rather than creating a secondary subtract feature.
  • As @Cesare mentioned use pattern face whenever possible. Pattern feature of a Feature set produces a large number of features. Pattern Face is good option as it creates less number of features. 

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.blend.PNG

  

blend1.PNG

 

Re: Downsizing of model size

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

It should be noted that the new file created by "heal geometry" will be unparameterized.

Re: Downsizing of model size

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

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)

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled