Have you ever needed a material database that has more than the standard materials that comes with SolidWorks? Over the past eight years I have created solid models for military and commercial designs that required accurate 3D models to send to our customers for weight and FEA analysis.I have weighed the actual against the calculated weight from SolidWorks and the parts were very accurate, 98-100% accurate. Major aerospace companies were pleased.I created my own material database based on the materials used in these industries
; it is available on my site for free download: Materials.[Updated 9/2016 ML]
Sometime in the near future, I plan on expanding the material database to include materials requested by other SolidWorks users and friends. [Update 9/2016 is now available at the link above. ML]
For whatever reason, watermarks are sometimes necessary, even on drawings.
Since SolidWorks has no watermark feature, and does not allow the user to change the order of drawing entities, a workaround is necessary. Here’s a method I recently discovered.(I am currently using SolidWorks 2007 SP3.1.)
- Open the drawing.
- Edit Sheet Format
- Use Annotation Note to create and place the text that will become the watermark.
- Edit the properties of the Note to adjust its font, angle, size, etc as desired.
- Highlight the Note and change its color using the Line Color function.For best results, assign a very light color to the Note.
- Right Mouse Button click on the Note and select Make Block and accept.
- Edit Sheet.
The Note will now appear underneath all other objects on the Drawing Sheet. This tip is based on the SolidWorks Forum discussion which can be found here:http://forum.solidworks.com/forum/messageview.cfm?catid=6&threadid=1989&enterthread=y
I have written an article detailing a more advanced method that will link the text of the watermark directly to a custom property here: Create a SolidWorks Drawing Watermark (with linked value).
UPDATE for SolidWorks 2013
SolidWorks 2013 now has the ability to set any annotation note on the sheet format to appear underneath all drawing elements to act as a watermark. The method mentioned above is no longer necessary to achieve the desired results. Please see SolidWorks 2013 What’s New – Display Note Behind Sheet.
To expand on my previous post, methodology in using SolidWorks should employ strategies that capture function (not just form and fit). This is true at the individual model level, and at the model assembly level. There are likely many ways to capture function within a model assembly. If used in a particular way, Horizontal Modeling can be employed. Other methods are Top-Down and Bottom-Up. Given the names of these methods, it is easy to see where the name “Horizontal” came from. The methods described here are for engineering environment where much of the design is custom or discrete parts, where similar componentry is rare. (As presented here, this is not the best methodology for creating model assemblies where componentry is very similar for a multitude of products, though some individual methods covered in this article might still be useful in that environment.) I don’t presume that what I’ve written here some sort of final say. My ideas have evolved over the years, and I’m sure they will continue to evolve as SolidWorks will evolve.
So, my preferred method doesn’t really have a name, per se. I use which ever methods are best for the particular task at hand, within certain given rules. For example, when working with model assemblies, it’s usually not a good idea to solidly use Top-Down methods. That is, do not create models at the assembly level and work down from there. It’s not that this is conceptually bad. It’s just that SolidWorks doesn’t do a good job at handing this method in the extreme examples. It creates relationships that are unnecessary and hard to detect during troubleshooting. (Yes, I realize this goes against the whole idea of parametrics, upon which SolidWorks, Pro-E and other applications are supposedly based.) However, some level of thought has to be put into building a model assembly that does resemble Top-Down methodology. To capture the function of an assembly within SolidWorks, an understanding of how the components interact with each in the real world must be considered. This is tempered by the need to create as much of a stable and editable model assembly as possible.
To do this, parts must be modelled with their most significant function as the core. This is the feature that is the most functionally laden. This is often the feature where the most important interfacing with other components occurs. Center that feature about the default reference geometry (the three default planes). Think about how the part is to interface with other parts. For example for a basic part, relative to the top view of the feature to its function, the feature should be centered on the X and Y plans, with the Z plane assigned to the mounting surface. Other methods also exist. The idea is to model the feature in the most functionally meaning way. If this is done consistently on all models within a model assembly, mating those components together using Horizontal Modeling methods will be much easier to execute and edit.
Once parts are modelled in this way, the model assembly is a simple matter. The reference geometry of that very same core feature can now be used at the assembly level. Before starting the design and modelling, determine the most significant part. This is the part that carries the highest functional burden. This can be the component to which most other components mate (such as a base plate). It can also be the component that interfaces with another model assembly or critical component. Other possibilities exist too.
Whatever type of part you decide is the significant component in your assembly, it is that part which should be first inserted into the model assembly. Align that model’s reference geometry to the three default planes of the model assembly, but do not mate the model to the model assembly’s reference geometry. In fact, never mate any model to the model assembly’s three default planes. Instead, fix the most significant component. This is the component to which all other parts will be mated, directly or indirectly. There are three main reasons for this. First, this functionally establishes the part as the core of the assembly. Second, this significantly reduces the chances that unnecessary or unintended relationships will occur in the assembly. Third, it allow the assembly more degrees of editability should realignment of this or other portions need to occur.
Only mate components to other fully defined components. All mating should be driven by function. Mate components to the core model as they would be in real life. This means using a logical combination of both reference geometry and feature geometry. If two faces functionally mate flush to each other in real life, then make the surfaces coincident in the model assembly. If a component is to be centered on a mounting plate, don’t use the mounting holes to mate the part together. Use the models center planes and the interfacing surface. Yes, apply the best method. Don’t use only features or only reference geometry. There is no preference between the two methods. Use the method that best captures the function. This may be counter-intuitive to some people. However, if it is understood that this is how a model assembly was built, I feel that this is the most intuitive methodology. Build the assembly based on function.
More important functions take precedent over lesser functions. If a model is fully defined, do not apply more mates to it to capture further function. This would be both redundant to the primary function(s), and cause over-defining errors very quickly in SolidWorks. This is part of the general rule for all modelling methods, avoid establishing unnecessary relationships. Having them will ruin any attempts of any good practices methodology.
By using this methodology (or combinations of methodologies, actually), one can capture a parts form, fit and its function within the SolidWorks environment.
Welcome to the launch of the SolidWorks Legion blog. Chris Saller, Chris MacCormack and Matt Lorono (I), have started this joint blog to cover all topics related to SolidWorks, from the very specific to the remotely connected. Help on troublesome topics will be provided. Opinions will be expressed. Examples will be provided. This blog will likely eventually touch on topics ranging from how to create shortcuts to examples in API, from information about users groups to product reviews for add-in products, and much more. Postings by each person are identified at the beginning of the entry. There are categories by which postings can be sorted and viewed. Tags can be used for this too. We hope this site will prove useful to all that visit.
Wanted to take a moment to say a few words about the technical school I am working for.
Northwest Technical Institute is located in Eagan, MN and has been around for 50 years as a private institution. The school is constantly producing excellent talent for the Drafting/Design and CAD technologies. Students are drilled for 16 months on ANSI/ASME standards, how to research complex problem for producible solutions, and how to use SolidWorks and Pro-Engineer using best practice modeling. I am currently teaching the Advance Modeling 1, Product Design for Manufacture and Sheet metal and Weldments courses using SolidWorks.
This semester the 4th Semester instructor and I are firing up a competition project that will put the 4th semester students in the team lead position. These student will design a glider in Pro-Engineer using all the available tools they have learned to model the farthest gliding distance. They will then outsource their detailing and manufacture of the design to second semester using email to coordinate the efforts and meet the project milestones and deadlines. The 2nd semester students will need to import the por-e models into SolidWorks (mean ain’t we) and detail them using many section views and inferencing dimensioning techniques. The school has done many competions like this in the past but this will be the 1st time we have one semester coordinate with another semester. This is shaping up to be very competitive and exciting. I cannot wait to see the frustrations, the pain and finally the results from this competition.
Â Anyhow, this is a brief glimpse into the school that I work at. I am always looking to those in industry that may have old project specs, ideas or info that may help to add even more realism to our curriculum so that our students are even more prepared for the industry. Also, forgot to mention, I graduated from NTI in 1997. My career has soared with their degree.
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