Model Assembly Archives - Page 7 of 7

How to use a Model’s Material directly on the Drawing

I should start out by saying that I personally advise against using the model’s Material value directly on a drawing (edit: for SolidWorks version 2008 and older; SW 2009 appears to have addressed some of the issues). However, below is the instructions to do just this.

First, let me bring up three problems when it comes to materials and the SolidWorks Material Database naming convention. One, the material names used in SolidWorks library are not correct. In fact, in many cases they are not even the common names for those materials. Two, for those of us who need accurate specification, the standards that define the materials are not mentioned of the library at all, making references to material incomplete. Three, the names of the materials are not capitalized, so they are not formatted correctly to be used directly on a drawing in the first place.

A solution to these issues is to change your library to add this info and correct formatting or create a new library to do the same. Another more common solution is to enter the information manually in a custom property within the model, then have that value pulled into the drawing via normal custom property linking, such as an annotation note with the following text: $PRPSHEET:”Material” or similar. Make sure to identify which view you wish the data to be pulled from, within the Sheet Property window.

If you still wish to use the actual model’s material value (despite all of the above reasoning), there’s a couple extra steps (also involving the use of custom properties):

1. In the model, create a custom property called something like Material at File>Properties>Custom tab.

2. For the value of Material property, just click on the down arrow of the entry field and select Material.

3. On the associated drawing, create similar custom property with the same name. (Again, make sure to identify which view you wish the data to be pulled from, within the Sheet Property window.)

4. For the value of the drawing’s Material custom property, type $PRP:”Material”

5. Create an annotation note that links to the drawing’s Material custom property. This will display the value of the model’s material directly on the drawing.

User Interfacing with SolidWorks (Make it faster, stronger, better)

Setting up one’s computer for using SolidWorks on a regular basis is a matter of personal preference in the extreme. There is almost literally as many ways to set up a SolidWorks station as there are SolidWorks users. SolidWorks provides many methods for user interface, including toolbars, peripherals, shortcuts keystrokes, menus, command manager and other assorted on-screen functions. The most important element is the human in the real world using SolidWorks in the electronic realm. The following is just some of my thoughts about things that can be done to make interfacing with SolidWorks easier.

Monitors

For me, I have found that two monitors works well. I set up one monitor as my primary where I run SolidWorks and other high-end software. I use the second monitor for reference and interfacing, to run such programs as Adobe Acrobat (PDF), PLM/ERP software, Internet, MS Office applications, commonly accesses desktop icons for these and other links of various type, etc. I also place less frequently accessed SoildWorks toolbars on the second monitor. Additionally, I place my SolidWorks command manager just on the edge of the second monitor where it is close enough for quick access, but removed from the main screen. This opens up space for my model view pane. It should be noted that I’m currently using SW 2007. Moving the command manager is currently not possible on SW 2008, from what I understand. I would like the ability to move the FeatureManager pane from the primary monitor as well. I hope this is a feature that will be added in SW 2009 or 2010. The goal for me is to have as much space as possible on my primary monitor dedicated to the view pane.

Also, I now recommend new widescreen flat LCD monitors of the 24″ variety or bigger. The prices have fallen drastically, while the quality has improved radically.

Mouse

I have found that a lot of people are perfectly happy with very low movement settings on their mice. This I cannot understand. It amuses me that people will drag a mouse halfway across their desk surface just to have access to a corner of their Windows desktop. They move their mouse 8″ just to click a toolbar icon, and them move their mouse another 8″ to get back to were they where. This is a bad time waster. It is also horrendous ergonomics, for which they will ultimately pay the price.

A mouse should be set to as sensitive a setting as needed to give the cursor arrow access to all portions of your monitor(s) within a very slight movement. I have my mouse set so that I can access any point on my primary monitor within a 2″ diameter of movement using a medium threshold. The threshold is the speed one moves their mouse to trigger faster movement of the cursor arrow. More detailed local movement of the mouse should also be as sensitive as possible.

This allows the user to control their entire desktop with very little movement. It increases speed of operation. It is also more ergonomic, being better for a person’s long term arm, wrist and hand health.

Shortcuts

To reduce the need to move the mouse around even more, use a lot of single stroke shortcut keystrokes. A lot of people may not like shortcuts for various reasons. I believe one of the most common reasons is that they are too hard to remember. However, they are worth remembering. The time savings from using shortcuts verses moving the cursor arrow around is tremendous. With the right sort of shortcuts set up, you can be working on one particular portion of your model and access several functions without having to move your cursor arrow back and forth from the toolbar back to your operating area. You can be in a sketch, switching from line to dimension to circle to trim, all without having to move your cursor arrow off of the view pane. This allows for much greater efficiency.

To make it easier to remember shortcut keystrokes, only add one or two at a time. When familar with those, as a couple more based on what you use the most. This allows you to learn/remember a couple at a time instead of a bunch all at once.

Of course, programming functions into the mouse itself will save even further movement of both your hands. This usually requires setting up shortcut keystrokes in SolidWorks that are then mapped to the peripheral. In this case, use very complex shortcuts such as CTRL-SHFT-F1. It doesn’t matter how complex because it’s still just a push of a button on your peripheral. Save the single stroke shortcut keys for other functions.

Strategy for Good Interfacing

A way of looking at interfacing with CAD software (particularly SolidWorks) is to think of functions in terms of how often you use them. The more often one uses a function, the easier and quicker that function should be accessible. One methodology is to work in the following way. The top 5% of functions used should be accessible with very little movement. If possible, they should be mapped to buttons on your mouse or other peripheral. The next 15% of functions should mapped to single stroke shortcut keystrokes. The next 25% of functions should be accessed through actual clicking of on-screen icons. Any remainder functions should be accessible through the pulldown menu scheme.

Also, if you find yourself using a series of functions routinely, then create a macro that accomplishes those tasks. Map that macro to a single or multistroke shortcut. Always be mindful of repetitive tasks and the ways they can be simplified to save time and improve ergonomics.

Knowing how to implement this strategy doesn’t come over night. It comes from working with SolidWorks over time. As you work with the software and pay attention to your own actions, you will become aware of what can be done to improve your efficiency. For me, if I repeat the same action over and over, I work to reduce the number of the steps it takes to perform that action until I get it to a point where it doesn’t bother me anymore. Use whatever means necessary to this end.

Jumping Toolbars, Cadman! (Toolbar changes not saved)

With SolidWorks 2007 and prior, most commands are available through on-screen toolbars. These toolbars are highly adjustable, both in content and placement. Sometimes, their adjustability in placement can cause issues that may make it seem as though SolidWorks isn’t saving toolbar placements. In my experience, SolidWorks does a good job at saving placements of toolbars. The issue many have with saving toolbar placement is often related to the fact that SolidWorks allows the same toolbars to be placed in different locations for each document type (drawing, model and model assembly).

It should be noted that some people do experience a real problem with toolbar placements not being saved. This problem is caused by a corrupt install or registry. To correct this issue, use regedit.exe to rename/delete the SW registry key (HKEY_CURRENT_USER\Software\Solidworks). This allows SolidWorks to establish a new registry key, and hopefully eliminate the corrupt information. (Note: this will clear all Solidworks settings, so use this method with caution.)

But, before that method is attempted, try this less drastic method first. As stated above, sometimes the issue is caused because different document types are using the same toolbar, but that toolbar is in different locations for each. This causes them move around when switching between document types. As they move around, they push other toolbars around too. Each time this happens, they can cause toolbars to shift into even more different locations. The solution is to have a drawing, model and assembly all open at the same time, then switch back and forth between them to see what jumps around. Adjust locations of the toolbars with each document type active. Switch back and forth from that document type to the other types. Do this for each of the three document types. Keep doing this until all toolbar locations are stable, no matter which document type is open, and to which document type is switched.

Then here’s the most important part: exit SolidWorks normally. It is the exiting of SolidWorks that saves the toolbar placements. The process can take about 5 to 30 minutes.

A side note, if SolidWorks crashes at any time after toolbars are changed, but before exiting normally, any changes to the toolbars will be lost! This is important to note, it is it a third reason why toolbar changes aren’t saved.

Introduction to SolidWorks Custom Properties

SolidWorks has something called custom properties. Many programs within Windows have file formats that include properties which allow the user to include some general information about the file without affecting its actual content. For most of these programs, there is a standard short list that includes fields like Author, Keywords, Comments, Title, and Subject. There is also a method that allows the user to create their own custom properties.

SolidWorks has simplified the process to create custom properties, and allows its users to utilize their values within the document via linked annotation notes. The custom properties are available under pulldown File>Properties>Custom tab. There are even shortcuts included that allows the user to create links in these fields to attributes of the document itself.

The advantage in using custom properties is that one can link to their values in annotation notes. This allows for automatic updates to annotation notes without having to edit them directly.

Here are the instructions to link a note to a property. (These instructions are from SolidWorks Help which can be found by searching titles only for “Link to Property”. For more detailed information, please see the Help.)

Start an annotation note.

In the Note PropertyManager (left pane) choose this icon:

-OR-

In the Note Properties dialog box, choose this icon:

Then,

Select the radial button that identifies the file from where the values will be linked. The most common choices are either the “Current Document” or “Model in view specified in the sheet properties” (for drawings).
View the available custom properties.
Choose one and then click the OK button.
This will add a tag to your annotation note that looks something like $PRP:”<property name>”. The annotation note itself will display the value of that custom property.

This can be used to automatically fill in data fields on drawing blocks based on custom properties and document properties in the model. It can also allow the fields to be filled in from a macro that is designed to provide those values. Linking annotation notes to custom properties can save a lot of time and reduce repeatitive drawing activies. However, before committing completely to using links to custom properties on drawings, one should look into the methods and reasons for this. They should also consider the pros and cons of each. I will go into detail about when and how to use links to custom properties on drawings in a near future article.

Create CAD Standards (SolidWorks environment)

Creating a drafting standards within a SolidWorks environment is an important task. The task may seem daunting to those of us who haven’t done this before, particularly if our company has no pre-existing documentation methods. These can be new companies, or companies moving from a lack of control into standardization.

Fortunately, there is a lot of help available. Actual drafting standards already exist. Also, many of us have been through this before (sometimes multiple times). ASME provides American National Standards for many of the areas that need to be covered. ISO provides international standards for these too, however I will focus on the use of ASME since this is what I used myself. On the other-hand, creating SolidWorks specific standards requires a little more reseach and upfront work.

Here are my very general suggestions for documents and tasks to create a company’s standard.

SolidWorks Templates (basic overview)
1. Create a basic solid model template. The setup within this template will become the backbone of everything within SolidWorks. This will be the most used document. Establish custom properties that detail the part. (Use of existing properties can be leveraged to simplify this task.) Creation of this first template does not preclude the creation of other solid model templates. Instead, it will be used to create any others. For details about templates, goto SolidWorks Help and search titles only for the words “document templates”.
2. Create a solid model assembly template. Many of the general settings of this template should be duplicates of the settings of the solid model template. Some planning is required. Determine the best method of assembly structure for your company. Several practices exist as guides, such as Top-Down, Horizontal Modeling, Bottom-Up, and Configurations. It is important to note that there is not one-size-fits-all method for all companies. Research each and make the determination based on company needs. Setup the assembly template to support the chosen method. However, do not become overly reliant on any particular methodology since situations may require flexibility.
3. Decide how the drawing templates will interact with solid models. This includes deciding to have any pre-defined views, use of custom and other properties, etc.
4. Create sheet formats and templates for each drawing size that will be commonly used. Include annotation notes linked to custom properties, such as part number, material, revision, originator, origination date, surface finish number and/or type, etc. See SolidWorks Help search for “Link to Property”.
5. If in a network environment, place the templates and sheet formats within a folder where all SolidWorks users will have access. Point all SolidWorks installs to this location. This can be done within pulldown menu Tools>Options>File Location>Document Templates and Sheet Formats.
6. Create a company standard for shortcuts and macros that speed up SolidWorks operations. Set up a network location for the company macros.
Create the following standard operating procedures.
1. SolidWorks Performancethat covers computer system requirements, Windows settings, SolidWorks installation, working folders, and standardizing files.
2. SolidWorks Best Practices and Standards
  - Solid models: discussing preferred methods for creating features.
  - Assemblies: cover methodologies (when to use top-down or bottom-up; and what part should be the primary fixed component) and how to avoid circular mating, etc.
  - Drawings: covering how to use templates/sheet formats, shortcuts, common macros, etc.
3. Drafting Standards, which can rely on ASME Y14.100 (umbrella engineering drawing standard), ASME Y14.5M (GD&T drafting standard) and possibly ASME Y14.41 (3D model drafting standard). List exceptions to the ASME standards within the procedure. If relying on these standards, make sure to have copies of them on hand. This will allow the procedure to be short and to the point. If not relying on a standard, this procedure can potentially be very long.
4. Source File and Document Control, which covers how to handle file management (SolidWorks files) and documents. Be sure to cover processes for control of SolidWorks files in folders and/or the PDM application. This may be a procedure that is supplemental the company’s general document control processes.
5. Revision Control, which covers how to revise engineering documents. This can rely on ASME Y14.35. If the company uses a ERP or PLM, this procedure may be supplemental to those processes.

For references for further research, check out SolidWorks resource links, such as weblinks that can be found here on Lorono’s SolidWorks Resources. Also, check out Blog Squad sites such as Matt Writes.