There are a few design criterion with hems that mostly deal with what is possible within the constraints of the bending tools. Unfortunately these are more "rules of thumb" than they are actual design constraints as every forming tool will have different requirements. For example, when hemming it is generally required that the length of the hem be approx. 10x the thickness of the material. This allows enough space and stiffness for the bending tools to do their work.
Hems of course can be created in more than one way, for example a miter flange can typically replace the hem feature. Of the four basic hem profiles (Closed, Open, Teardrop and Rolled) each can easily be created as the profile of a miter flange. Here though, as is mostly the case, the preformance of the hem is better than work arounds using other features. At the same time though Solidworks can have problems creating mitered edges for a hem.
Above, even though the two features have the same profile and gap distance, the software chooses to miter the corners differently. The one of the right with an open corner is created by a hem. Even though the miter flange is clearly more resource intensive, designing the correct corner is more important and for that reason I've found that in most of my parts (and on the sample tests) the mitered corner feature will be the preferred route.
A bend creates two types of stress on a material. Compression on the inside of the curve (creating a shorter inside distance) and tension on the outside of the curve (where the material is stretched longer than it's original).Zoom in on the above picture and you'll see that the total length of the flanges and bend on the outside is 4.08". Below the total length of the flanges and interior bend is 4.00". This seems obvious except when you consider that this piece starts out as a single flat piece of material with the top and bottom surfaces being identical in length. This means the material deforms when bent (due to the stresses mentioned above) but there is one cross section of the material that stays at equal length. This is called the "Neutral Axis". The relationship between the distance to neutral plane and overall thickness defines the K-Factor.
K Factor is used in defining the bend allowance, thus by using bend allowance tables it is possible to automatically set the K-Factor for defined materials (See gauge tables). Standard K-Factor's can be found from your sheet metal supplier, online, or through real world testing. It is only one of the ways bend values can be determined. See the others.
Gauge Bend Table
I've spent some extra time looking at these values because a changing K-Factor appears as one of the questions on the CSWP Sheet Metal Sample exam provided by Solidworks. To change the value for the entire part just select the primary "Sheet Metal" feature and in the property manager for Bend Allowance select K-Factor and enter the value.
This is only one of the ways the bend values can be calculated. See others
Gauge Bend Tables
This is only one of the ways the bend values can be calculated. See others
Gauge Bend Tables
Using a bend allowance the flat part will be longer than the distance of each flange combined.
Using a bend deduction the flat part will be shorter than the distance of each flange combined.
This is a slightly more involved calculation that is defined by how a material deforms. A bend creates two types of stress on a material. Compression on the inside of the curve (creating a shorter inside distance) and tension on the outside of the curve (where the material is stretched longer than it's original).
Gauge Tables: Gauge Bend tables are one way to define bend values. A little up front leg work in setting these up can save a lot of hassle and many small errors. Because values are unique to the material a separate table is required for each material.
The most obvious application of this is in material selection. If there are only a few stock sheets to choose from to design then most of your default values will not have to change. Solidworks knows this and allows for a one time setup to save time, just like it does in other parts of the system (design library, toolbox). Once selected in the "Sheet Metal" feature all values will automatically be imported. The table used can be changed even after a part is fully modeled (although doing so will likely cause rebuild errors). To change this you can access the table in the "Sheet Metal" . To further consolidate information it's even possible to create a Gauge-Bend table that links all of these values. When using a Gauge-Bend table an additional selection will be available under the Bend Allowance.
Above is the feature manager for a single BEND, where the bend allowance can be modified (see here again the option of Gauge Table is present because this part has an active Guage-Bend table). There can be many of bends defined within a single Flange feature, which means even if more than one Bend Allowance value is used it is still possible to have a neat tidy feature tree. In general (and in this case) a smaller feature tree results in a more efficient design in terms of rebuild time.
So now the big questions.
How do I setup or change a Gauge or Gauge-Bend Table in Solidworks?
Solidworks comes with a few basic tables that are stored in folder as part of the install (fittingly called "Sheet Metal Gauge Tables"). Take a look at the Sample Steel table and it is pretty easy to figure out how to add values. This is all done in Microsoft excel and most cells contain notes. Using the samples as a template it's easy to do a quick "Save As" to get a new copy, then just change the values needed. Note that below I have excel open on top of Solidworks for viewing purposes you can also edit the table directly in Solidworks using Edit>Bend Tables>.
Check out the Sample "Bend Allowance" files to a joint gauge-bend table. Another note here, make sure the units selected in the table correspond with those in the part file. Although it's possible to circumvent this it is much easier to recognize and alter items that are causing issues. Personally I spent about 30 minutes trying to figure out how to setup the fields, with no results. Once I used matching units it was easy to tell where my changes were propagating out to.
My best suggestion is to play around with these and make sure you know how to change each field. Reading the help files and looking at this site can help but nothing replaces actually making your own table.
Closed Corner: Saying this feature is "more detailed" is misleading. Rather it's an easy and intuitive way to complete a design while avoiding some hassle. A corner could conceviably be closed using a series of Linear edge flanges, tabs, etc. all with odd profiles. Rather than waste time creating this though SW does the legwork for you. This feature works similar to the "Extend Trim" popular in sketches. Fairly straightforward, just select the features you want to form a corner, select the corner type, and let SW go to work. The only variable here is the gap distance which is typically driven by the type of welding that will be used (or rather the quality of the welder be it human or machine). Consult a sheet metal supplier for the best options.
The welded corner feature is as much cosmetic as it is functional. Not only does it add a nice looking weld bead to seal a corner (if "add texture" is checked), it also easily denotes a weld feature on a print. The best list of weld symbols I could find freely available helps to properly denote these items in conjunction with GD&T, although a google image search turns up some good results as well. Some of these change but in general that guide works but for applications where precise notation is important an actual copy of the standards is helpful as well.
This one is very basic and is essentially another way of making a Fillet or Chamfer. In a series of quick testing the sheet metal option (Break Corner) was preforming slightly better than a Fillet Chamfer. This makes sense due to the extra options allowed in the Fillet Feature. Break corner the software will only select edges that are of the material thickness, or perpendicular to the flat sheet metal. These corners are then filleted prior to any bends, as they would be when a manufacturer creates their flat profile. Other edges that may be filleted are more difficult to create in manufacture, genreally requiring grinding or a more sophisticated profile cutting (stamping). Here is seems Solidworks understands what corners are mostly changed and has built a custom property just for those making things easier on a desinger who is unfamilar with the manufacturing process.
The sheer scope of knowledge presented at Solidworks World leaves me with a daunting task, even more so when the audience following online is looking for a piece of everything. Thankfully the beauty of the social media age is that you can be a part of things to. Anyone with suggestions or comments on what I should be looking for, who I should be talking to, what sessions will be interesting or anything else just drop me a line via a comment or tweet.
I am truly looking forward to this experience, thanks again to Solidworks.
Solidworks World on Twitter
Solidworks World on 3D Engr
Get to start figuring out what is going in the morning. **If you want an invite I've got a few just post a comment**.
So far the first few study sections for the CSWP-Sheet Metal have been fairly easy. I'm expecting the exam to be similar to the CSWP where these basic features defien most of the geometry of the parts and having a solid grasp on them sets you up for success. Still more to study though, for a full list of my review see the base post back at CSWP Sheetmetal.
Even though this feature is rather simple, there are some details which are important both from a modeling and manufacturing standpoint. The first few items (Radius and Gap Distance) are essential but mostly only need to be entered once per part. This is because the Base Flange function creates a feature that stores this information.
The flange angel is also easy to determine from prints, drawings or models and can be put in just as easily.
The next feature is a little tricky, Flange length, this is due to how the feature can be measured. Length can be measured from the inside or outside edge of the radius and the difference in the two is obvious (see animated .gif below).
On prints this should be dimensioned in the same way the icons in solidworks are shown, in measuring though this can be difficult with calipers or rulers. If accuracy is paramount getting the correct value of a "Virtual Inner Sharp" is nearly impossible as it is difficult to determine where the bend of the material actually starts. Although a machine shop with good communication skills will get clarification on these types of values, if they are ambigious, not all will and you can be left cutting down or scrapping whole lots of components.
The same issue appears on the flange position, what may seem like a simple selection during modeling can greatly effect fit. Generally having an error here will cause measurements to be faulty by a value relating to the material thickness. For 12 guage steel that's .105", multiple by a second wall and a simple enclosure can be off .21" (get a full guage chart for sheet metal on the web). What's more any items dimensioned in relation to the walls can also get screwed up easily during fabrication. Imagine designing a nice little encolosure for a circuit board and realizing that all mounting holes are out of place by nearly 1/4 in, not good.
Take the time to talk with a fabricator about how they prefer to see a print (everyone has different opinions here) and make sure if there are issues to explain them in notes on a print. Even engineers with a thorough understanding of GD&T practices will appreicate an extra note if it saves them losing a batch of parts.
So it's easy enough to start a linear edge flange, but how do you know what to make? First let's look at the call out used on drawings. Drawings for sheet metal parts are needed in a variety of phases but the basic one is the flattened part. The default is a series of variables if you replace " with <> you'll get:
"bend-direction" "bend-angle" "bend-radius"
or something like
So in the bottom the dashed line denotes where the material needs to be bent UP (bend-direction. The two resultant faces will have a 90deg (bend-angle) angle between them and the bend will have a radius of 1mm (bend-radius). These values are gathered from the Property Manger of the flange feature. Checking the "Use default radius" button will use the radius provided in the "Sheet Metal" feature.
By just selecting an edge Solidworks will extend a flange along the entire edge for whatever distance is selected in the "Flange Length" section (either blind or up to).The other portion of the property manager that is intriguing is the "Edit Flange Profile Button". Select this and a property window appears to show the software is in Sketch mode. Here any sketch features can be used to create the geometry of the flange. Although this should be a closed profile it's worth noting that this profile does not need to be just a simple rectangle.
Adding geometry here to avoid additional features also improves performance, sure it isn't a huge impact for a single feature but propagated through a large assembly these types of little changes can make a significant impact.
Above are the statistics for a rebuild with the hole made as part of the flange sketch. Below is a rebuild with a single closed profile flange sketch and the additional cut (Extrude3).
There are more parts to the property manager tab but each of them will be reviewed in later posts. For now I feel confident in identifying and modeling linear edge flanges of varying profiles.
1. Existing web presence. 3DEngr.com may be a new site but I got started here to explore the world of 3D design and what better place to do that than at Solidworks World. My RSS reader also currently looks like this:and if selected I plan to personally meet and interview the writer of each of these.
2. Been there. Good or bad it's nice to know what your in for at least a bit with such a huge confrence. Having been to Solidworks World 08 (San Diego), I realize the enthusiasm of attendees and recognize the impact a trip can have on all. Last time around I met a few names who I still follow online. Specifically, Ben Eadie who did a great presentation on a home built 3D scanner (which later appeared on his blog). Matt Lombard, I only spoke with Matt briefly about user groups but he handed me his card for Designstuff.com and blogs which led to my google feed reader eventually looking like it does today. Matt also gave me another name, Mike Puckett, at the time the head of the Los Angeles area user group, Mike got me involved in the user group (although I haven't been to the LA/OC group in a few months due to a extended stya in another state)
3. NOT Been There. After a great 2008 trip SWW09 in Orlando fell the same week as a tradeshow I had...in Anaheim. With no way out of it I had to follow along online so I know the audience. It's cold, the holidays are over and you want to see pictures of cool products, hear about the crazy new features being added to SW11, get vicariously drunk at the CSWP event, and bump virtual elbows with Richard Branson (2009) and Theo Jansen (2008).
4. I'm a Local. I live in West LA about a 35-40 minute drive (or up to 55.33hours in traffic) but will be staying at a close friends during SWW to avoid said traffic. That puts me within a 5-iron of the Angels Stadium; an easy commute over to the convention center means I'll actually be getting a good seat for the general session. Unless the video camera has some serious zoom this is necessary even with a media pass as the place fills quickly.
5. Relate to attendees. I've worked with Solidworks now as a Student, as an engineer where it was the existing CAD package, as an unemployed engineer through the ESP pack, and by convincing a new employer to get a seat (making me a "CAD Administrator"). I don't plan to take one of the session "tracks" and will provide a robust overview of what is offered at SWW10 and no presenter will be safe from this correspondents camera.
6. I need a GOOD boss justification letter. Oh sure, the one of the SWW10 website is helpful but I used up a lot of my "look what this can do" karma on getting him to purchase an actual seat of the software. Being tapped as the correspondent makes it easier to swing.
7. I'll throw a Beet. What, blatantly pandering for support from a larger site is frowned upon? With the boys over at Solidworks Legion pushing for their guy (CTopher will be my first interview BTW) I need some help.
8. I'll tweet like it's my job. Although technically since I will be contractually obligated it *is* my job. Get ready to see #SWW10 in your twitter client of choice with all sorts of amazing links and tips.
9. I read all the rules and agree to them. Sure this might be a minor point but it should count for something. I'm over 21, not from Brazil, China or Quebec, can meet with SW Social Media Manager before the show, don't care about the odds of winning, and have no family or professional ties to Solidworks. We're a go.
10. I'd really like to, please. My mom always said to try asking nicely. Being the correspondent sounds like a great opportunity and I believe I have the skills needed to be successful. So, Please let me be the Official Solidworks World 2010 Internet Correspondent.
Thanks, and hope to see you there (or if you're not going I hope you'll be following along online.) And if you have visited this site and liked anything it'd be really great to see a comment here or directly on the Solidworks Blog.
Recently I found myself looking at some of our current products, which are made of sheet metal. My experience with sheet metal is minimal and as I go about modeling these parts I want to use all the features I am used to. Having worked primarily in plastic part design this is difficult as many sheet metal features are difficult to show. Thankfully the built in sheetmetal features will solve this problem but I'll need to figure out what they all mean and how to use them. So now it seems time to do some studying. The goal here will be to pass the CSWP-Sheetmetal Exam. From 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.A sample test for the CSWP-Sheet Metal exam is provided by Solidworks as a study tool but
first up I'm going to run through the tutorial built into the software. Here is what it says I'll learn.The CSWP-Sheetmetal Test covers a few other things as well. I'll review them in subsequent posts (linked below) but first what's to learn from the tutorial.
The first thing to note about Sheetmetal is that there are a lot of variables. This is evident by the start of the design tree. To start any sheet metal part a base flange is created which, after first created, actually inserts 3 features into the feature tree. These contain information for the material being used (thickness/gauge), how it will bend (bend radius), the base sketch, and a layout of how the part will fold flat (as sheet metal is made out of a flat sheet).
Having these features also sets up some new parameters in other functions. Linking features to the thickness relates back to the value saved in sheet metal, this can be seen in extrudes and cuts. The rest of the tutorial course helps you build out the rest of a basic part and create a drawing for it. Most features are used but can be glossed over by entering simple values in a few places. Taking the time to understand each one individually seems more productive so I'm going to take a look at the required features one by one. Again, direct from Solidworks, those are:
Finish up the study, take a look at the practice exam and it's time to get a certificate.
Exam features hands-on challenges in many of these areas of SolidWorks Sheet Metal functionality:
As I have gone through studying for this test I keep finding more and more helpful resources, not one to hide good information I will include them below. Some of these are outdated tutorials but still helpful.
Solidworks Resources for teachers- Sheet metal.