Drawings performance in SolidWorks can be instantly improved with some simple settings. Changes or by using open modes. Here are our top five tips to help boost your drawings performance. To review the performance of a drawing performance evaluation can be used from the evaluate tab. Here we can see the open and rebuild time, as well as isolate specific views which might be more demanding. We can view statistics to see a breakdown of the drawing elements which might be affecting performance. Any view that involves cutting the model will demand heavier. Calculations and therefore increased loading times. Examples include section, remove section and crop views. For shaded views consider using shaded without edges for the display style. Since edges are the most demanding aspect to display. Converting views to draft quality is another method to improve performance. This will give a graphical representation of model data rather than loading in actual model edges. We should look to convert any demanding views to draft quality by selecting them and changing the property manager setting. Make sure that your PDF export settings are set to high quality lines and edges to ensure that you have a suitable print quality. The view palette represents a significant portion of the rebuild time. So this can be cleared by using the cross to reduce the open and rebuild time of the drawing. The refresh button can bring back the view palette at any time. Be aware that if an assembly part is already performing poorly, a drawing will also. Our certified SolidWorks Assembly Modeling Course is a great way to learn more about optimising your models for performance. Component interference can also make a large impact on performance, especially when sharing section views as there is not a single defined edge and SolidWorks must calculate the new edges. Be sure to use the interference detection tool in the Assembly Evaluate tab to review models and fix any problems. Our second tip is to review system options. Here are some useful ones. Firstly, under drawing settings we can deselect automatically populate the view palette with views. While the view palette is helpful for importing views. It takes time to rebuild. And can impact performance. Consider turning this off and loading the view palette manually as it is needed. Next, look under the display style settings for drawings. Here we can set the default edge quality levels for shaded and wireframe views. Draft quality views will demand less performance but should not impact exported PDFs as long as our export settings are set to use high quality. as long as our export settings are set to use high quality. The performance settings and the drawings are also worth reviewing. Turning off or modifying settings such as show contents when dragging can make significant improvements. We can also force drawings to open in detailing mode by default from here. This is something we will learn more about in the Open Mode section of this video. General SolidWorks performance settings can be looked at since these will also apply to drawings. Choosing to load components in lightweight under performance settings can speed up assemblies and the drawings that reference them. Large assembly settings are particularly useful to look at for assembly drawings, since these will also impact the general performance of assembly environments. Document properties are file specific, but we can adjust them in a blank drawing file and then save a new drawing template to allow future drawings to use the same settings. Image quality is an important document property to consider. The further to the right that the slider is, the sharper your edges will appear, but consider moving the sliders to the left to improve performance. Under the performance tab, we have the option to save model data. Under Detail Mode settings. In most cases, this should be turned off. If you're not planning on using detailing mode. If the setting is enabled, SolidWorks will save extra information and increase the save time when you're saving in resolve mode. This is just so that there's more information available to you when working in detailing mode. We'll learn more about this in the next section. When selecting a drawing to open in SolidWorks, we're going to be presented with three possible open modes. The first of these is resolve mode. This simply loads all the model data into memory. It is the default and it's going to take the longest to load. However, there are no limitations on editing. Secondly, there is lightweight mode. This only loads a subset of model data into memory. The information can be loaded as it is necessary if commands such as model license need to be used. You can fully resolve a lightweight drawing at any time by right. Clicking a lightweight view and clicking set lightweight to result. The third option is Detailing Mode. This opens without loading the model data into memory. Commands that require model information are limited in this mode. But some drawing view types can be created and annotations can be added. If the previously mentioned save model data setting was ticked before the last save. More options are going to be available to us. We can also selectively open certain sheets for drawing. This can be useful if we're only editing one aspect of a multi sheet drawing. Any sheet not selected will be loaded in a quick view which only allows viewing and printing. Open options and settings are covered in detail on our three day drawings course. Find out if there's a class running near you on our website. A major factor in drawing performance is where files are being loaded from. Where possible we should work locally. If we're fully loading a drawing file into memory. The associated parts and assemblies must also be loaded. As a result, if we were to open a drawing from a network drive. The open time will become dependent on network speed. Ideally, load files onto a solid state drive before opening for optimal speed. Beyond the steps discussed in this video, you can verify that your hardware is up to standard at the following website. Generally, you're going to be looking for a minimum of 16GB of RAM, a high speed CPU processor, and a modern Certified professional graphics card. Certain window settings can also be impacting your performance. For example. If you're using Windows, check that your power plan is set to high performance in power options, or you may be limiting your SolidWorks performance. For more tips and tricks for improving your SolidWorks drawings. Check out our other videos or our blog which is regularly. Updated with new tutorials and advice.