material Archives - SolidWorks Legion

Return of Ctopher’s Custom Material Database

Custom materials in SOLIDWORKS are important if you are using materials not included in the default set. Around a decade ago, Chris Saller compiled a bunch of such custom materials from varies sources based on requests and submissions from many different people. This list is informally known as Ctopher’s Custom Material Database, “ctopher” being Chris’ handle.

Various versions of this file have been available on now long-gone websites over the years. Well, the material database is finally back and bigger (better) than ever! Chris has complied a new version in SOLIDWORKS 2016. This new version has many new materials. The new database is now available directly on SolidWorks Legion in the File Downloads tab as Ctopher’s Custom Material Database.

There are two methods to point SOLIDWORKS to use a custom material database. The easiest method is described on Ctopher’s Custom Material Database download page. Below is a slightly more advanced method which should also work on networks.

To point SOLIDWORKS to make the materials in this database available:

1.To use, place custom_matls_091516_sw2016.sldmat file into an easily accessible folder, such as S:\SOLIDWORKS Shared File\Custom Materials. The folder is your choice, based on your network and operational set up.

2.Start SOLIDWORKS.

3.Goto Tools>Options…>System Options>File Locations. In the Show folders for dropdown, select Material Databases.

4.Select Add button. Navigate to your chosen folder, such as S:\SOLIDWORKS Shared File\Custom Materials.

5.Select OK button.

6.Repeat for all instances of SOLIDWORKS within the network that need to access this database.

To use the custom materials:

1.Open any part file.

2.In the Feature Tree, right click on Materials and then select Edit Materials. “Custom_matls_091516” folder will be on your material list.

4.Click on desired subfolder, such as Copper Alloys.

5.Click on desired material to view properties.

6.Click on Apply to apply that material to your part.

7.Click on Close to return to your part.

Ctopher’s Custom Material Database

Ctopher Custom Material Database

Author: Chris Saller, et al.

Author’s website: ctophers home

Ctopher’s Custom Materials Database allows you to add many materials to SOLIDWORKS which are not currently included as part of the default installation. Materials range from ceramics, metal alloys, plastics, crystals, and even magnets. Current version was created using SOLIDWORKS 2016.

This database is provided for reference only, being based on tertiary sources. The database is not an official offering from DS SolidWorks Corp. in anyway, nor is DS SolidWorks Corp responsible for any content or how it is used. Information within the database is not guaranteed to be correct or accurate. Information within the database was submitted from multiple persons and sources. No one is responsible for the content of the database. The user of this database uses it at their own risk. The user is responsible to crosscheck all information for accuracy to a level that suits their own needs.

The database is a combination of materials used in aerospace and military applications, and SolidWorks users around the world submitting material properties to add to the database. The material mass properties have been tested with actual parts on a scale.

To allow SOLIDWORKS to use the materials in this database:

1.To use, place custom_matls_091516_sw2016.sldmat file into C:\ProgramData\SOLIDWORKS\SOLIDWORKS 201x\Custom Materials folder.

2.Start SOLIDWORKS and open any part file.

3.In the Feature Tree, right click on Materials and then select Edit Materials. “Custom_matls_091516” folder will be on your material list.

4.Click on desired subfolder, such as Copper Alloys.

5.Click on desired material to view properties.

6.Click on Apply to apply that material to your part.

7.Click on Close to return to your part.

Download Custom_matls_091516_sw2016.zip

SolidWorks 2010 Multiple Materials in Multibody parts

In the SolidWorks 2010 Beta 2, there was only one entry in the What’s New file under Parts. It is a rather modest statement regarding the fact that each body within a multibody part can now be assigned its own material.

You can assign different materials to individual bodies in a multibody part. The material assignments are used by mass properties, drawing section views, and SolidWorks Simulation.

That’s it! That’s all the Beta 2 What’s New file said. It didn’t even say how to add material to different bodies! (Beta 3 did add some information, but not a lot.) Even the embellishment regarding where the material information is used doesn’t do this new capability any justice. Think about it! Are you kidding me?! SolidWorks now allows us to give a different material to each body within a multibody part! Composites can now have material information included in the part file! No more guessing, estimating, averaging out properties! No more funky assemblies to try to get around the previous limitation! For example, the user can now model a part and its coating in one file to accurately run FEA simulations!

OK, so how does one add material to each of the bodies within a multibody part? A general material can still be specified in the same way as before. RMB click on the Material heading within the FeatureManager of the part, then choose Edit Material. This will assign a material to the overall part. The steps are just a little different to assign material to a specific body. LMB click on the Solid Bodies folder. RMB click on the body which will have the different material, then pick the material for that body. When complete, the Solid Body will have its material listed underneath within the Solid Bodies folder.

Ctopher’s Material Database – Update

The new ctopher’s Material Database is here! The long anticipated new update of my material database.

The new database version 070508 has been updated with more materials.

Because of conflicts with some of the materials between SolidWorks 2008 and older versions, we created two versions. One version is for 2007 and older and the other is for 2008 and newer. Both are included in the same file.

Also added is a text file with instructions.

Thank you to Matt and others for your help and contributions.

Chris (ctopher)

Download page: ctopher’s Material Database

(*.SLDMAT)

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.