CSWP: Mold Tools

Just looking at what is next on the list to study for. I've got a few side projects I plan to work on but there are lingering vouchers for the Mold Tools and Surfacing tests and figured I may as well study for them with what time I do have.

Having worked for an injection molder for a little over two years the Mold Tools exam seems like it would be right in my wheelhouse. However, due to the workflow and design process at our shop it was rare that we used mold tool features other than cavity. Most other features were created using non-mold specific features. Typically we would import the part into an existing mold base, luckily this is one industry where the leaders have realized that getting CAD data out there for customers to work with is beneficial. DME, one of the big players in mold bases and mold components has data for their entire product line, though a login is required. Working from these files it always seemed the best route was to extract and build onto the existing base rather than model a generic mold and then merge it with the stock base.

So on to the test, Solidworks says the test covers the basic mold tools and will "help to aid a user in the completion of a robust mold design in an efficient manor". Although this may be the case it's silly not to point out that this test does nothing for showing a user knows MOLD DESIGN. Rather this shows that a user can model a mold. The specifics of mold design, allowing for stable molding and efficient mold fabrication, are not the core of the exam. So here is what it covers:

Exam features hands-on challenges in many of these areas of the SolidWorks Mold Tools functionality:

All of the above should be reviewed for the exam, but I will also take a look at a few concepts that are core to good mold design, and at least one feature that is left off the above list

  • Core Tool
  • Part Draft
  • Ejection
  • Undercuts and side pulls
  • Wall Thickness
  • Materials
Of course the sample exam for the CSWP Mold tools (zip) will also help. More things may come up along the way and as they do they will be added. Again I've found a lot of information on Youtbue as well, as I find/upload more they'll be placed in this playlist.




Get more Mold Tools Training

Practice with Solidworks: Modeling random items

Tutorials of creating random sheet metal parts is fun and all but sometimes it's nice to practice modeling something else. Water Filtration systems are fine, but what I am designing professionally is limited in feature scope. As I built out a library work is becoming more and more a drag and drop routine, which is rather nice and allows me to focus on actually managing projects (ie. make sure suppliers/vendors are happy/informed). So whenever I have a few minutes I grab something from my desk or around the house and see how it can be modeled to try to branch out. The user group I attend (Los Angeles/Orange County) has competitions where the entry is just this, model anything. Models are then put up for a vote and the winner is the one that gets the most votes. There is no criterion for voting, no judging scale, just show a picture of the item to a room full of users and let them decide what they like most. In the past I did well with a corkscrew.

Recently, during a few hours of down time, this is what I saw on my desk.Just a small staple remover. Nothing to detailed to model but getting the fit/form just right still takes some thought. I also wanted a model that I could use for rendering practice. Making such a basic component seems easy, and although my first few render attempts came out okay I'm still not happy with them. The lighting is not quite right and having the part float in mid air is not providing the results I'd like.

CSWP: Sheet Metal Certificate

After all that time spent reviewing I managed to grab a few free hours to take the CSWP Sheet Metal exam. The first go around I had a system crash halfway through when downloading some attached material. Thankfully I sent an Email to Solidworks certification folks and got a speedy reply and solution from a great guy over there, Avelino. The second go around there were no major issues and I managed to complete the 15 question exam in 77 minutes (you are allotted 90). No perfect score this time, although when looking back now I see what I likely made my mistakes, not so many that I failed of course and the result was this little certificate.CSWP Advanced Sheet Metal SpecialistCertificate Chris McAndrewSo what does the certificate mean. According to Solidworks
The completion of the Certified SolidWorks Professional Sheet Metal exam shows that an individual has successfully passed a skills test that demonstrates their ability to use the sheet metal tools inside of SolidWorks. Employers can be confident that an individual possessing this certification understands the set of tools inside SolidWorks that will aid in the design of sheet metal components.

Not bad, I think the test could have been a bit more comprehensive but it did a good job of requiring the use of each feature type. Due to the precision required for answers (usually within .2%) it also verifies that a user can pay attention to detail or rather has the ability to trouble shoot for slight variations.


Now what? Mold Tools are in my wheel house but Surfacing has always been fun....

Flatten- CSWP Sheet Metal

Whoa, it's the last feature of Sheet Metal. Things here are pretty basic, select the feature in the tree or unsuppress it to get the flat pattern of the part.

All of the flatten feature options are spelled out nicely in the Help Files, although none of them should effect the results for the exam. The one option that may make things easier to manage/understand is "Merge Faces". In the formed part each wall has it's own face, but in the flat pattern all of these faces are coplanar. Identifying the intersections make it possible to measure flattened bend lengths (can also be measured as arc lengths in non-flat part).
This also provides an easy way to grab values for bends that will assist in verifying the bend calculations reviewed earlier.

The other option noted is the Sketch transformation. This will appear as a folder at the end of the Flatten feature tree ONLY if there is a sketch that must be transformed AND the part is currently flattened. Solidworks will use any sketch not linked to a feature. The original sketch if shown will still appear floating in air (as seen in the picture). The transformed sketch can be used in drawings of the flat pattern.

That is pretty much it for studying for the CSWP exam. Reviewing one more time, redoing the sample test and then it's time to get certified.

Unfold and Fold- CSWP Sheet Metal

The fold and unfold commands are unique from the flatten command in that they are time dependent. The Flatten feature appears at the end of the tree and can be suppressed and unsuppressed to view the flat pattern, but the fold and unfold features can appear anywhere in the tree. As with other Solidworks features that means that the software reads them in the order they appear in the feature tree.

It is sometimes the case that a feature must be punched over a bend. During the manufacture process these punches and cuts are created while the part is in the flat state, thus when designing them it is important to locate and model the feature while the part is flat.


1. Insert an Unfold feature and select the bend that the feature extends across.
2. Create the required geometry (typically a cut or hole)
3. Insert a Fold feature and continue modeling
"Collect All Bends"

For the Unfold feature "Collect All Bends" will select every bend in the part, essentially mimicing the flatten feature. In Solidworks 2010 Sheetmetal parts can contain multiple bodies. When this is the case "Collect All Bends" will only select bends on the body connected to the "Fixed Face".

When unfolding the "Collect All Bends" button will find and select all bends that are currently "Unfolded", even if they were unfolded using multiple unfold features, assuming they are still on the same body.

When folding and unfolding selecting a "Fixed face" is important. If the "Fixed Face" of the Fold is different from the "Fixed Face" of the unfold part orientation will be thrown off. This could effect the part orientation in Assemblies depending upon the mating features.

Solidworks World 2010 Calendar of Events

Gearing up for Solidworks World 2010? There is plenty to do, and I don't want to miss anything. With some of the sessions filling quickly I've only made it on the wait list though it appears this is happening mostly in the "hands on" sessions where computers are limited. After seeing Matt West's post on the Solidworks blog I realized I'm signed up for both of Phil Sluder's sessions (@Sluder on Twitter). It seems Phil has been working hard on his presentations and I hope to get some time to speak with him afterward as he is one of only a handful of people who have attended every Solidworks World.

I'm still finalizing my itinerary and surely there will be some game time changes but here is the calendar of events I'll be attending.

If you want to get in on some extra fun start following @CbMcAndrew, @SolidworksWorld, or @MatthewWest on twitter and I'll let you know when the details of the Tweetup are finalized.

Forming Tool- CSWP Sheet Metal

Form tools are used during the manufacturing process to create unique features on parts. Punched holes, vents, indentions, ribs and plenty of other functional items can all be modeled this way. Typically once a tool is made it is best to design future parts with the same features to eliminate the need for more tools this can reduce time to market and lower the overall tooling costs for new designs. On the software side of things, having a forming tool created eliminates the need to recreate features and sketches.

Form tools are saved as specified files .SLDFTP (Solidworks Forming Tool Part)

The work flow for creating a forming tool goes like this
1. Create the geometry of the forming tool. This should result in a single body.
2. Add a "Forming Tool" feature and define the faces
3. Save the file as a Forming Tool (File>Save As>.SLDFTP). This should automatically bring up the folder where forming tools are kept
4. Open a new sheet metal part
5. Create all needed features
6. In the right side bar>Design Library navigate to the forming tools folder.
7. Add the form by clicking and dragging from the right side property Manager
8. Position the sketch as necessarySolidworks already has a few form tools saved in the install files. For a better example of how to work with these tools I suggest trying to add and edit these formed features and tools.

With Solidworks 2010 it is possible to make multi-body sheet metal parts. Below I added the body for the default "Bridge Lance" feature, in red. This is the body used in the .SLDFTP. The sides of the body are denoted as "Faces to remove" in step 2 above. The result can be seen.

I also found it interesting to note that editing a form tool will NOT edit all of the parts. At least in the test I ran, saving form tools in SW 2010 SP 0.0. The formed items are created based upon the geometry of the tool at the time of creation. If the tool is changed and saved later the changes will not propagate back, rather the feature must be manually edited at each instance. This is likely to improve performance, forming tools are relatively basic and accessing another file to define them is less efficient than simply copying the geometry and features.

Sketched Bend & Sketch Rebuild Times- CSWP Sheet Metal

A sketched bend is one of the easiest ways to change an existing sheet metal part. In a similar fashion to the "Jog" command a sketched bend can create a feature without adding any material. This helps to maintain a conceivable flat pattern without having to create too many relation rules. A one line sketch will take care of defining the feature but positioning it is key for component fits. Thankfully the bend positions are laid out in an easy to understand diagram.

So then it comes to defining this one line sketch. Recently I read a post by Matt Lombard where he busted the "Fully defined sketches are faster to rebuild" myth but I thought this would be a good tool to get some more evidence. For a Sketched bend even a simple 1mm long line will cause the same feature as a fully defined and extended line. Both of them simply tell the program where to make a bend. So what difference does it make to fully define where the bend goes. Here is a simple line section used to create a bend.

Total rebuild time was .06 seconds undefined. And now below is the fully defined version. You can see the rebuild time for the sketch has increased significantly (0.00sec >>0.03sec) and the feature (0.06sec>>0.08sec) for a total rebuild of 0.11sec fully defined.

Interestingly HOW you fully define the sketch also makes a difference. Above I used model snap to relations to link endpoints of my line to the midpoint of a wall. Using value dimensions instead allows the sketch to rebuild in 0.00 seconds:







So what is the result of this result of all this to the model? Nothing aesthetically, all three produce the part shown below.


The point here is not that leaving sketches undefined is a best practice, quite the contrary. Fully defined sketches are good practice and having them will alleviate a lot of headaches and errors. But not all dimensions are created equal; for a sketched bend the length of the line segment does not matter. It's distance from other edges is mostly likely the important dimension and thus allowing automatic solutions, such as snap to relations, may not be the most efficient way to design the part.


Stump the Chumps at SWW10

It's never to early to start deciding on your itinerary for break out sessions at Solidworks World. Back by popular demand, after a one year lapse, is "Stump the Chumps". This panel of Solidworks power users will be available to answer all sorts of technical questions. Submit a problematic design or part prior to the session and there is a good chance these guys show you multipel ways to solve your problem.

Questions can be submitted via email stumpthechumps @ gmail dot com. Or check them out on Twitter with the handy hashtag #StumptheChumps.

Solidworks World CSWP Event

I've started to take a look at some of the breakout sessions and events to attend for Solidworks World 2010 and see how busy my days will actually be. There is a lot to be excited about but the one I'm most looking forward to is the Certified Solidworks User Event. This will be my first time attending as I had only passed the CSWA last time around. Luckily there are a few teaser videos and some details from the forums:

For SolidWorks World 2010 we have teamed up with the guys over at Team Associated who are industry leaders in remote controlled cars and trucks. When you walk into the party venue at SolidWorks World we will have multiple tracks set up allowing anyone the chance to drive one of their awesome R/C trucks. You will also have the chance to compete to win your very own R/C truck to take home with you. There will also be professional drivers on hand showing all of us their driving skills.

Of course we will also have a fully stocked beer and wine bar, as well as plenty of food for everyone to eat. Don't forget that CSWP's also get a $100 discount on the admission fee to SolidWorks World. You can register for SolidWorks World and get more information over at the SolidWorks World 2010 Page.







There is still time to take the exam before the conference, or sign up for one of the on site testing sessions that occurs before Monday night. Need some help passing the CSWP exam, take a look at all the other CSWP tutorials and walkthroughs.

Jog- CSWP Sheet Metal

The jog feature in sheet metal is yet another tool that simplifies design features. Many times a 2 bend step is required for mounting, to avoid other features, or create a simple wall and using the jog feature combines them into one item.

A few of the benefits of jog.

In the feature manager there is a selection box for "Fix Projected Length". By Clearing this length the software will ONLY use the material that is already existant. Now if the dimensions of the jog require additional material to be added an error occurs.
This is a huge help considering that all sheet metal parts must be flattened. If there is a limited amount of material available the jog feature (with Fix Project Length cleared) will lock in this design intent. Skip this step and solidworks will still let you design a part, and even flatten a part which can not be created. Take a look at the images below, see something wrong? You should. This part can not be created from a single flat sheet of material, look at how the flat patten overlaps itself.


So when do you use a fixed projected length? Use it when you can add material, on the outside of parts. This is great for in context modeling of multi body parts or assemblies.

Above I've taken a tab that would have caused interference and moved it while still keeping it's length in one direction. The alternative to using the jog feature here would be to Cut>Edge Flange/Tab>Edge Flange Tab or Cut>Miter Flange the part. Even though the jog feature is system intensive on the rebuild the relations required to capture the design intent are much easier to input using a jog and it keeps the total feature count down.
 
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