Working With Large Files in Autodesk Inventor

IMAGINiT Tricks Tutorial: Don't get stuck waiting for your files — update your settings and save time now.

Colors and Finishes. Some colors and finishes can increase the file size as well. Adding a finish such as a reflective color will also increase the file size. Colors that are "flat" increase the file size the least, so consider using those where applicable.

Consider purging any unused color style definitions, especially for common parts. Keep in mind as well that each time you change a material or color in a part file, the style definitions are cached in that file. Each time this file is used in an assembly, the unused definitions are multiplied and impact the memory.

To properly purge these unused definitions, go to the Manage tab, in the Styles and Standards panel, click on the Purge button, save the file.

Assembly Files

You can also speed up load times for assemblies by limiting or minimizing the number of constraints you use. Build upper level assemblies by means of sub-assemblies. This eliminates or minimizes the number of redundant calculations Inventor has to solve and complete for that upper level assembly to build.

When working in larger assemblies, open the Application Options dialog box and be sure to deselect the following options:

1. Enable Relationship Redundancy Analysis
2. Enable Related Relationship Failure Analysis
3. Features Are Initially Adaptive

Adaptivity. This is a double-edged sword. Adaptive parts are created within the assembly when you reference an edge or feature of a mating part. This is a great feature to use on parts that you want to update when their mating part changes and can be very useful early in the design process when changes are happening quickly. But at the same time these adaptive parts can bring an assembly to its knees when used extensively. Generally you should disable the Adaptivity option once the parts are fully created. If and when you need to edit it, you can re-apply this feature until your edits are done.

You can disable this option in the Application Options dialog box. Under the Assembly tab | In-Place Features heading, de-select the check box for Enable Associative Edge/Loop Geometry Projection During In-Place Modeling. To disable Adaptivity on the fly, right-click the part in the assembly browser and de-select Adaptive in the pop-up menu.

View Representations. If you find yourself in a large assembly, whether it be in file size or physical size, setting and using View Representations can greatly improve time spent navigating by selecting the needed View Rep as opposed to using the orbit command. This becomes evident when you have a very simple or quick edit to make and you need to navigate to a specific section of the assembly and in turn waiting for the graphics to play catch-up.

Level of Detail (LOD). Opening a large assembly can be a time consuming task, especially if you have numerous assemblies to open. This doesn't have to be the case. Earlier we discussed a part file's End of Part Marker, assemblies do not have an EOP marker, but they do have a default set of Level of Detail. Like the part file's EOP marker which reduces the file size to the minimum, utilizing the All Parts Suppressed Level of Detail will accomplish the same results for assemblies.

In the Assembly browser, expand the Representations folder, expand the Level of Detail node, and the default LODs are:

• Master: No parts are suppressed
• All Components Suppressed: Everything suppressed
• All Parts Suppressed: All parts at all levels suppressed
• All Content Center Suppressed: All Content Center parts suppressed

Select either All Components Suppressed or All Parts Suppressed, depending on your needs and save the assembly and check the file size. Whereas these default LODs are close to being "all or nothing," you can also create your own LOD that specifies what level of parts you have active upon opening the file. You are not limited to the number or the names of your LODs.

This can also be done at the Open File dialog box if you rather operate that way. In the Open File dialog box, select the Options… button, and select the appropriate level of detail to open in the Level of Detail Representation pull-down menu. This option may be a better fit for you in that not all your assemblies may be very large where you'll need this option.

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