Trim/Extend Command - CSWP Weldments

When creating weldments one of, if not THE, most important dimensions is the length of each segment. Depending on the end condition (flat/butted) this may be the only value needed to actually manufacture the cut list of a given profile. For this reason the trim/extend tool is extremely useful.

If structural members are created in the same feature (using groupings) the software will automatically trim each member according to the end condition rules applied. However when items are created as separate features, either because they are different profiles or the work flow deems it necessary, the trim will not occur automatically.

This image highlights two members. The one on the right has been created as a group in the feature "Structural Member1", the trimming of it is already done. On the left is the member created in "Structural Member2", as can be seen the profile has been extruded along the length of the path even though it over laps any members. It is important to understand when automatic trims occur and to verify this prior to production because at times the visual nature of the model make make it difficult to see the overlap.

There are a few selection options as to what surfaces can be used to trim a weldment. Items can be trimmed up to a specific face, which is the typical case for most profiles that will get straight cuts. Weldment trim with face
An almost identical result can be achieved by using a trim with body. This requires the total body to be selected, but here selecting a "simple" end condition will do the trick.Trim works well enough, but in certain cases it will wind up extending a feature as well (see the tool name Trim/Extend!). In the below image horizontal member at the bottom initially does not come to a point, it is flush with the other corner. When using the Trim tool and faces the extension is added. This same issue appears many times when trimming corner member that will require more than one trim. Each configuration of corners will have a solution that is best and when in doubt the manual trim (see below) is always an option.

If however there is a need for a more complex cut, to help in welding or to show off the abilities of a cool laser cutter, a member can be cut using a body or with coped ends. This will provide a more detailed end and is essentially an "up to" cut or extrude.

If the trim tool is not getting the job done a cut can be created manually to trim a member. This is the same as any other cut but because it is a weldment choosing which bodies to cut becomes more critical. This is an option at the bottom of the feature manager for a cut, simply select the member or members needed and everything is taken care of. Even with an end condition of "thru all" the cut will only cut through the selected bodies.
Weldment trim using cut tool

Cut list items are automatically linked to their length. This is a property that will show up in a drwaing and denotes the length. At a user group meeting recently the question arose as to what length gets pulled in. After doing some testing it seems Solidworks will provide the length as the maximum point to point distance along the normal of the profile. This is just to say it lets you know how long to make the initial cut. Even if the cut is curved as in the manual cut example above the longest segment is always the value Solidworks pulls in. Below are a few examples to show this.
Weldment Trim Coped LengthAbove is the coped cut, below a simple cut. In the cut list table the length feature is obviously different. In this case the difference is equal to the radius of the corner fillet on the item as the coped member has to cover this distance as well.

Weldment Simple trim length
This last example shows the same members but this time with a very awkward manual trim. The 15.81 is the value of MAX distance along the profile normal, ie from the furthest point of the circle to the flat face at the opposite end.Wedlmetn Cut length for complicated cuts in Solidworks
The cuts and trims are a basic tool but some of the more complex member intersections can cause issues. Knowing what each tool does can help create a proper cut, ensuring that a manufacturing cut sheet is accurate and no items will be cut too long, or worse, too short.

More details about the weldment tools can be found in the rest of the CSWP Weldment review overview.

3dVia Shape Initial Reaction

It would be nice to have a free, lightweight, platform independent, user friendly, powerful CAD software that works for everything. Unfortunately most CAD packages only deliver on a few of these criterion. In an attempt to broaden my knowledge, and to find out what is out there I started looking at a variety of 3d modeling and design software. This post is only one in a series and is intended to give my initial reaction when researching, downloading, installing, and the first use of each. For a compiled list of reviewed software check the overview post.

3DVia Shape

Right off the bat I like Shape for one reason, it's free. As a part of the Dassault Systemes family 3dvia is an attempt to get 3D everywhere. Bernard Charles, the CEO of Dassult, has openly admitted he is making a billion dollar bet with the company generally surrounding the "server in the cloud" approach to 3D modeling. Though Shape is not nearly as powerful as some of the other Dassault offerings it was one of the first to pioneer this crowd sourcing approach with a directly built in option to publish models to the website.

So how useful is this software? It really depends on what needs to be designed. For production manufacturing Shape is not going to cut it, but to develop some ideas, or teach a new user the basics of modeling in 3D it may serve a purpose.

Coming from a background with parametric, or history based, CAD prog
rams Shape is a whole new beast. This can be both good and bad.

Installing 3dVia Shape and System Requirements

3dVia Shape can be downloaded and installed fairly quickly. The installer is just the first download, more files are downloaded once the installer is run but in contrast to some other software installs (I'm looking at you Solidworks) this is a very quick process. For me, clocking around 1.2Mb/s download, I was able to be up and running with 3dVia Shape about 15 minutes after I initially clicked the download button. The requirements for it are also less than many
other higher end software.

  • Microsoft Windows XP SP2, Server 2003 SP2, or Vista both 32 & 64 bits
  • Windows Internet Explorer 6.0 or higher, or Mozilla Firefox 2.0
  • 250 MB or more hard disk space
  • 1.0 GHz processor (2.8 GHz or faster recommended)
  • 512 MB memory (1 GB recommended)
  • 128 MB video card (256 MB recommended) supporting OpenGL 1.1 (Open GL 1.5 recommended) with OpenGL 3D hardware acceleration enabled
  • 1024x768 screen (32-bit true color recommended)
  • High-speed or broadband Internet connection
  • 3-button mouse recommended

What is Shape all about. Interview with Cliff Medling of 3dVia

3DEngr: Who is Shape designed for, Students/Professionals/Hobbysits?

Cliff: All three. And, we could include gamers, and K-12 students as well. Anyone creating 3D models.

3DEngr: In your opinion how does Shape stack up against other CAD packages in terms of Price vs. Functionality?

Cliff: 3DVIA Shape was never meant to be a CAD tool, but a conceptual or quick modeling tool. CAD tools include functionality to bring a design to production, where Shape was not designed for this purpose. The advantage of 3DVIA Shape over other CAD tools is the ability to create something very quick, that I can immediately be shared on For example, let’s say I just envisioned a new children’s toy design, and I want to share the idea (that is currently only in my head) to someone quick. I would not want to build this model in a CAD package, as it would take too long. I can use the simple features in Shape to design the toy (not to any specifications). I would publish the toy design to, and send the link to others, who could view it in 3D on any computer with internet. If I wanted to eventually produce the toy design, I could add detail in within a CAD application, like SolidWorks.

As for a comparison with other 3D modeling applications, we have tested 3DVIA Shape against other similar packages in focus groups. Those new to 3D modeling found 3DVIA Shape much more intuitive and easy to use. I must also add that my two boys (aged 6 and 9) use Shape every week. It’s easy for children to understand with minimal instruction. I just posted a video... about this very thing:

3DEngr: Shape seems to require a unique approach to building models, specifically compared to history based modeling. When first learning shape did it take long to transition your modeling techniques?

Cliff: 3DVIA Shape is actually built by the same people who designed CATIA, the PLM 3D modeling tool used by the top automotive and aircraft companies worldwide, so we have some of the best 3D modeling designers working on 3DVIA Shape. I could reiterate from my last statement about how easily children can learn 3DVIA Shape. It’s a great application for those new to 3D.

3DEngr: How did you learn, what helped you learn shape?

Cliff: I have used so many 3D packages over my career, so Shape was very easy to pick up, it really is very intuitive. We have plenty of learning materials on our video and tutorial channel: to teach those new to Shape.

3DEngr: You mentioned that you still modeling things regualrly and your main package is Shape. Are these mostly hobbyist things like the remodel and lamps to show your wife or do you use it to express design ideas or engineering ideas to professionals

Cliff: Exactly, I can build models so quickly using 3DVIA Shape, that’s why I use it most. It would take much more time to design any object in other CAD packages. If the object I was creating was very detailed or I needed precise tolerances, I would use SolidWorks.

3DEngr: Where are the limitations in your eyes, What items will you NOT use Shape for?

Cliff: If I was eventually going to build a physical prototype or if I needed a highly detailed 3D model, I would not use 3DVIA Shape, it was not built for that. It may be a good first concept, but not the final product.

One more advantage I wanted to mention about 3DVIA Shape: There is a lot of talk about “the cloud” in design. is closer than most companies to using the cloud, as we have proven that users can collaborate on their designs, and keep their designs online, and not on their desktop. Every 3D model I have created using 3DVIA shape is located on the server. I can access the model from any computer, by just logging in to I believe this is the future of 3D design, and 3DVIA is already there.

One other note I wanted to make: is useful to anyone who creates 3D models, whether it is a manufacturing engineer, a 3D artist, designer, etc. We accept 3D models of most formats. You can store any 3D model on, and share easily with others, who can view them in 3D using our 3DVIA player – our lightweight FREE plugin. It’s a great way to share and collaborate any 3D creation.

3DEngr: Thanks for taking the time to answer these questions Cliff. As he said all of Cliff's models can be found here on the 3dVia library.

Tutorials and Learning 3dVia Shape

This is one of those areas where Shape shines. Because it is a free platform there is no reason to package tutorials in the software and slow things down, rather they are posted online. Hosting videos on the 3dVia site serves a dual function. First it is a great reference for learning the software, the tips and tricks of 3dVia offer a sampling of the functionality and provide examples for the workflow required to get specific shapes.
Second, it serves as a great marketing tool when items like the car model are shown.

More Shape training Videos can be found on Youtube.

The biggest trick to Shape, and the reason I think it Shape should be introduced to a younger audience , is knowing geometry. Without any real dimensioning tools available to lock in lengths or arcs or lines it is important to have a way to define each segment. For example, an earlier post too a look at spirals in Solidworks. The key was that the system was able to define a spiral for me, but the thought process that went into defining a spiral was more "what can this feature do" rather than "what actually is a spiral". With this in mind it took a few minutes to come up with a way to create a spiral
in Shape.Helix modeling in 3dVia

Here are three equal circles on 3 planes. By first sketching a few line segments and using the midpoints the planes were created equi-distance apart. 3dVia has a nice set of snap to features that allowed me to make perpendicular and equal segments. The mid plane circle came next and then few more line segments to attach all three. Lastly an arc which requires 3 points and would function as the helix. By snapping to the vertex opposing sides of two planes I had the basic path but the 3rd point was the key to all this hassle. Here I snapped to the midpoint of the other segment that stretched between my first two planes.
Creating a profile at one end of this helix allowed me to use the push/pull feature along the path. There were some issues getting the profile to essentially "sweep" along the path likely because the profile created was not actually on the path initially. This is where the ability to insert standard planes and references would come in handy. After copy/pasting this segment a few times to create a coil from one revolution something was wrong. The tangency of the start and end points meant the curve was not creating a helix. When the profile swept along the path it started out a little bit too tangent and the finishing tangent was not the same. Copying the component using the mirror flip further enhanced the non smooth surface. This can be overcome by trimming the start and end portion or further reducing the segment to a working portion or by creating an entire helix, which is next on the list of things to try.

First Actual Model

I decided to try my hand at making something that was at least identifiable. A quick glance at my desk revealed a pencil jar, and I went for the most basic one in there. This model too all of 25 minutes to create and most of that was spent resizing things to get the right look though I did discover a few handy tools. Here is what helped me

Alt key- I hate that every CAD tool uses a different functionality to rotate around 3d space. At first I thought it was necessary to actually click the rotate tool in shape but the Alt key works as well. It's annoying that complete pan/zoom/rotate can't be done with a mouse though because it means two hands are used. How am I supposed to eat a sandwich and admire my cool models if I need a second hand.

Copy Paste/Space Bar and Shift - Hitting shift during copy paste of model items maintains orientation. Space bar allows the point of insertion to be changed. Both are shown in the handy help menu that is always aparent at the top of the screen.

Shape is not without it's bugs either, and one of them was apparent in my first modeling attempt. When opening Shape it requires that you sign in to the server. It seems that the server will however log a user out after a set time. So if you take a while to create a model and then try to upload it there is a server error. A google search turned up a forum post which had a workaround to saving but not knowing that my files are always secure is quite a concern. That being said, while modeling a second item the software completely froze again (to their credit I'm not running on the greatest system, granted I am above the recommended mins but I also was running 2 and sometimes 3 CAD programs as well as a few other things while working in shape). This time however my model was maintained, it seems a local copy was kept or somehow stored away. Akin to the new "cloud" version of things previewed at Solidworks World this year, my model was given back to me in exactly the state it was when the freeze occurred.

Next up was something work related. The lack of true dimensioning is a fatal flaw, meaning Shape will never make it's way into our production drawings but for showing off an idea or two it could be useful. Actually, the lack of history makes it an ideal candidate for throwing together ideas. Pushing and pulling surfaces without having to worry about slow rebuilds and lots of errors, that is something worth hanging around for. This is the model of a basic pressure vessel, again no engineering principles are applied here but as a representation of the vessel it does an alright job.

Last was something more fun. Without any children toy ideas on hand the next best item was one that contained slightly more geometry and is easily recognizable. Still a small and basic model this iPhone model helped to gain some familiarity with the tools used in Shape.


Shape has its limitations, and did not run flawlessly on my system, but when it comes to easy to understand programs it delivers. Most of my modeling will continue to be done in other programs but the ease of working in shape and the quickness of download make it a good option if I ever am on another system and want to quickly express an idea.

End Caps- CSWP Weldments

End caps for weldments are rather basic. This is one of the areas where the software knows what typical design intent is going to be, and a feature specific to that task has been created. Not having worked directly in an industry where weldments are regularly used I have no idea whether or not this is an accurate representation of the manufacturing process. Other functionality in Solidworks does this (I'm looking at you mold tools) where although it is a nice idea, most engineers or designers have an alternate way that more closely resembles their fabrication process.

Still though, this is likely to be on a weldment exam as they love making sure you can tweak the settings of these rather basic tools. So let's see what can be done.

To start an end cap simply click the End cap icon. A feature manager will appear asking for a face selection. Choose the end face of the component to cap.
Play around with the depth value and thickness ration values to see what each does. Below I noticed that setting an offset value that is greater than the part thickness causes a failure as should be expected.
The offset value is measured from the outside of the part. A ratio can also be used by clicking the check box.
Cap direction: Above the outside end cap is shown as it extends beyond the edge of the part. Below an inside end cap was created. This keeps total component from extending out where someone can smack their shin and instead cuts off an equivalent depth from the end of the main component. If for any reason the face at the edge of the weldment is used for any other mating entities this function can create errors.
Chamfering the cap is also an option and is definitely a candidate for being on the test. Visually a chamfer is easy to recognize and the value of it should be clearly noted on any print or attached model. Simply type in the value and the chamfer is added.
The end cap feature also changes the cut list. Because the cap is an actual piece it creates another cut entirely. In addition, the segment that is capped will be renamed to reflect that it is capped.
If multiple End caps are created they will be noted in the cut list with their corresponding numbers. Below I have 2 end cap features that create a total of 3 end caps. The first end cap is denoted as End cap1[1]. The 2nd and 3rd end caps are on a single section meaning only 3 components are a part of End cap2.

The naming scheme of these also caught my eye. The cut list will dynamically update to the name of the feature in the tree. To be certain of this I tested it out by only renaming the feature and this was the result.
If by chance a member needs to be capped on both ends, but with caps of varying values, the member itself will not be name for both of them. Rather the history of the tree will take over and the component will be name for the last feature that acted upon it. Basically this is to say that not every end cap necessarily requires 2 corresponding members. This all may sound a bit verbose but with the need for an accurate weldment cut list (it's part of the required knowledge for the CSWP weldment exam) I found it important to note.

Weldment corner modification - CSWP Weldments

One of, if not the, most important portions of a weldment to control is the corner. In production an error of cutting can create a nightmare for a welder. Not only will these errors look bad, but a welded corner is typically the first place to look when a failure of the part occurs. With that said, here are the options on modeling these items.

Group End treatments or Single Corner
When adding weldment parts to a file the first step is grouping the components together. There are a variety of different ways to group but the important part to remember is that a group can only create intersections between two components. If a corner will have 3 or more weldments meeting at a point it will need to be controlled over two groups. In the image above the corner treatments on the group scale can be seen in the left feature manager pane. Highlighting the each group in the list will allow each to be edited separately. However, if a corner is more complex or needs a hands on approach it can be edited directly. Simply click on the pink dot at the corner vertex to bring up a selection window. In the above image it is seen on the right. The selections here will override any in the group.

The basic types of joints are easily selected. With the real time preview it is easy to see exactly which two components below to the same group. Here the miter joint is for the items with more pronounced blue lines. The third leg is controlled in another group.

Butt joints are the other main type. There are two options given in the main feature manager but really they just change the orientation.

Trim Order

When there do happen to be three legs, or the global settings for a group are creating unintended corners the corner can be overridden. Again by clicking on the purple dot a "Corner Treatment" window will pop up. Here you can switch the treatment or the order. In the above picture there are three legs that all meet nicely and EACH ONE is mitered. Because there is more than one group this can get slightly tricky. The software will look at the lowest group order first, and miter/butt those joints, then it will look at the next one. So lets say that third leg was in group two, and it was solved after group one, it would wind up looking like a butt joint. See, by the time it gets solved the corner is already full of 2 other components.
To solve this problem we want BOTH group 1 and group 2 to be looked at when solving the miter. In the single corner treatment box you can look at both groups (the arrows around the 1 of 2 in the above image will toggle). Instead of solving them in order change the trim order of both groups to be the same. Now the system will look at all three components when making the corner. This is how you can get the three spears meeting type corner seen in the first image

Simple CutDepending how the cuts to the extrusion will be made a simple corner may be all that is available. These are simple straight line cuts.

Coped CutIn contrast to the simple cut, the Coped cut creates a more detailed part. With some high end laser cutters it is possible to treat the edge of each length so that there is almost no gap. This can reduce the width of a required weld and greatly increase the strength of such parts. In modeling it also looks a lot nicer as all edges will be complete and the areas of white space or background that would have been filled by welding wire anyways will be sealed. When making a cut list and drawings though these edges can become a nightmare. Again, unless a sophisticated CNC machine is going to use this data directly the headache of odd lengths etc should be avoided.

On the exam I am sure it will be important to identify a few corners and knowing what each feature does will surely help. For more review on the CSWP Weldment exam check the main post.

Placing the Weldment profile in the Weldment profile library - CSWP Weldments

Although most of placing a weldment profile in the library was covered in an earlier post, I wanted to go through it on a separate post. There are a few key things to remember here.

1. Know where weldments are stored. If you're like me you've had a few service packs and maybe even multiple versions of the software installed on your system. This can lead to having more than one folder that *should* contain weldments. If you've got a CAD manager who properly updates all template files that is great. If not no worries, just find out where those folders are and point SW to them. Under Tools>Option>File Locations select Weldment profile from drop down. Every external file reference can be found this way, including all Design Library folders, note that the design library folder is NOT necessarily the same as the weldment profile library. Usually these are stored on a global server, which helps eliminate reference problems on multi user systems, but if you are running a personal or home license you can slap a folder right on your desktop.
2. Saving to the Library. File>Save As will get you most of the way, then select the file type "Lib Feat Part (*.sldlfp). Once this file type is selected the browser window will automatically navigate to the design library folder. Again this is the DESIGN LIBRARY FOLDER noted in step one which is NOT necessarily the weldment profile library. If they are not one and the same, navigate over to the weldment profile library manually.
3. You're STILL not there. The main folder denoted in step one doesn't even contain the actual profiles. Instead in contains more folders. To figure out how these are organized I need to try adding a weldment. I created a new part file with a single line and tried adding a structural member. That brought up the property manager below on the left. Below right is the file structure of my weldment profile folder. It is easy with this view to see how the folder names relate. The top level is the Standard. Type is a subfolder inside of the Standard folder, and the Size is the actual file name inside the Type folder.

4. Done? The file is saved to the profile library so it should be ready to go right? Nope. If you try adding this profile into a weldment part now you'll get this error. As with all library features the actual feature needs to be added. So open up the profile file and take a look at the feature tree. Right click the feature that contains the profile.

Select "Add to Library", as seen above, I am only selecting ONE of my two sketches here. A small green arrow will now be added to the feature that looks like this . This will only add the feature selected and for weldments ONLY one should be added. For other design library items more than one feature from a part can be used. However if you try to create more than one profile in a single weldment file this error will pop up when adding it to a part.That's all of it. Now check out the rest of the weldment reviews.

The condensed version.
1. Select the weldment profile folder.
2. Save a profile to the proper folder
3. Right click the one (and hopefully only) sketch in the file and select "Add to Library"

Fun with Coils and Springs

Extrudes and cuts and go a long ways to creating some cool parts, but they can not do everything. I have always known about the Helix tool in Solidworks (Insert>Curve>Helix) but recently a few things prompted me to realize the limitations of Helix's. The first thing that happened was I had to create a model that would have required a helix that curves. When creating a helix however it is only possible to do so in a single direction. Variable pitch and diameter option are helpful in creating more complex helices but still they are lacking. The second catalyst, which rang clearer, was a comment at a breakout session I attended at Solidworks World. In the Stump the Chumps session, which includes a who's who of bloggers, power forum users, and SW employees, a question arose that could be solved using a helix. Charles Culp (the leader and guru of the Solidworks forums) and Matt Lombard (the Solidworks Surfacing Bible author) both agreed that using curves was NEVER the answer. Charles stated that any time he creates a helix his next step his to create a 3D sketch hit convert entities, turning his curve into a 3D sketch. Matt seemed to think any curve required can be created using surface tools (surprise!) and that these surfaces are more predictable and more easily controlled. So, let's see what all of these options are.

Simple Coils

The picture below shows a few basic coils. Initially all of these look the same, and geometrically they are. Each is 4 inch diameter, 5.25 inches in high coil. All three contain 5 coils, and have a wire thickness of .25inches.
Image 1: Identical Coils
Simple Coil Options
So how are these parts different, in the method of creation of course. The image below shows the expanded feature tree of each component.

Fig. 1
Simple Coil or Spring option in Solidworks
Method 1 (far left in Fig 1): Sweep twist along path. This one is easy and all it takes is a little known option in the "Sweep" command. Select twist along path and voila! You never actually define the path of the coil but for simple items it works.

Video 1: Coil using Profile Sweep-Twist Along Path

Method 2 (center Fig 1): Sweep using helix as path. In the video I have already set up the helix at a 270deg start angle to ensure that my profile sketch on the right plane will piece the helix at the end point. A 3D sketch would also solve this problem if I didn't set the angle correctly, but we can see here where Charles and Matt may take issue with curves. You do however get to create the path of the coil, and visually seeing it before creating is helpful.

Video 2: Coil using Profile Sweep- Helix as Path

Method 3 (far right Fig 1): Sweep using surface edge as path. Create and view the path of the profile, check. Easily locate the profile on the vertex of the surface, check. By creating the surface and selecting the edge at the path more folders are added to the tree to deal with the surface body. This is an easy fix, simply select and hide the surface after the fact, unless you like looking at the fun slide-like geometry. This option is the most resource intensive but also the most predictable and as things get more complicated this work flow looks like a great option.

Video 3: Coil using Profile Sweep- Surface Edge as Path

Curved Coils

I noted at the beginning of this post that my prompt for looking into coils included the need to create curved coils. For example purposes I created a coil that is circular. The below pictures show two options of a profile twisting around a circle. To help illustrate I made the circle a solid body as well.
Image 2: Curved Coils

The issue I was having initially was that when creating these curved coils my original work flow always caused my profile to get compressed. Unless the profile is kept normal to the path it is sweeping over this "smushing" effect kept occuring. The "twist along path normal constant" sweep option was not helping any. Below is a visual of what was occuring.

Image 3: Curved Coil Problems
On the left, my initial sweep work flow was getting smashed. Using the existing surfaces it was simply guesswork (or rather, a severely complicated hand calculation) to be able to get the profile in such an orientation that it would stay normal to the sweep path. On the right, by using the surfaces to create my path it gave me the ability to add a plane. Once the path was created I added a plane that was normal to the path at a point, than it becomes possible to have the profile piece the path at a normal.

Step by Step: How to create a coil using a Surface Edge path
Step 1: Start out by creating a single circular sketch. This will be the major circle around which everything happens. Mine is dimensioned to 20 inches.

Step 2: Next create a line segment on a perpendicular plane. Make sure the the end of the line segment pierces the original circle.

Step 3: Insert a surface sweep. Use the line segment as the profile, and the major circle as the path. Under the "Options" select Twist along path. Insert the number of twists required. Mine is arbitrarily picked at 13.

Step 4: Next insert a plane. This will be used to sketch the profile of the coil. For my relations I selected the edge of the surface and made the plane perpendicular. I also selected the origin.Step 5: Below the plane is now inserted.

Step 6: Select the plane and start a sketch. Draw a small circle and dimension it with the coil wire diameter. Select the center of the circle and Ctrl-Click the edge of the surface. A property manager will come up to add relations. Select Piece. Because the plane is perpendicular to the sketch surface this means the center of the whole is pieced perpendicular.

Step 7: Insert a sweep feature. Select the circle profile created in the previous step as the profile. Select the surface edge as the path. The perpendicular pierce relation will be maintained along the sweep path keeping the profile perpendicular to the path at ALL points. This is key to not "smushing" the resultant coil.

Step 8: The Surface body still remains. Locate it in the feature tree.
Step 9: Right click on the surface and select "hide", the icon will now appear clear.

Step 10: Finally I created a final sweep to add perspective to my images. I created a new profile but used the same path from step 1.

The same theory can be applied to many sweeps. A further look at the surfacing tools will help to create more intricate surfaces edges that can be used as paths.

Rebuild Statistics for Coil Methods

Because there is nearly always more than one way to create a part I make it a point to occasionally look at the rebuilt times for the various methods. Typically the multiple options are similar to each other, reordering features, changing one feature to another, etc. For the current exercise the change is not so small. Not only are extra features required for the surface method, but entirely separate bodies must be created. With that said below are the build times for the

Fig. 2: Statistics for sweep NOT using surfaces for path

The above image shows the statistics on the rebuild of the "smushed" coil seen in the left panel of Image 2 and 3.

Below is the rebuild for the coil seen in the right panel of Image 2 and 3.

Fig. 3: Statistics for Sweep using Surfaces for path
It is then obvious that, as expected, using surfaces significantly increases the rebuild time.

Note: It was announced at Soildworks World 2010 that Solidworks 2011 will contain a feature that allows a user to lock a model along the feature tree to prevent the entire model from rebuilding. This "feature lock" tool will greatly impact the ability to quickly make changes to complex models.

What Can Helix Do for You?

So all of this surfaces business is fun, but that's not to say the simple helix option should be completely ignored. The ability to have variable pitch and diameter helices is a powerful tool and can go a long way in simplifying a design. Many standard springs can be created using only a single helix feature and a sweep. Add in a powerful design table and there is essentially no reason to even open a file to create a new spring.

Above is an example of a variable pitch (and variable diameter) helix. Playing around with the settings here is a good way to figure out what can be done. I've actually seen something similar to this sweep in a consumer device. The application I am thinking of was a water bottle that had an obnoxiously long straw that encircled the container.

I could fill another twenty minutes of scrolling texts with more examples but they would all boil down to the same basic principles. If I missed anything here feel free to drop me a line as I truly am looking for all the ways to create coils and I would love to add some more content.
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