Weldments are a part of the Solidworks software that are intended to be used for parts that will require welding. It leads to reason then that small details, such as welding gaps in lengths, should be handled in an easy and intuitive fashion. Sure enough, one of the built in options when inserting weldment members is the option to include a gap between the components.
In this first image the feature manger can be seen with a value input for G1. This value inserts a gap between all member in the same group. Because it is intended to be a weld gap there is an upper limit on the value of this field which is set to one inch. If a member needs a larger gap one can be created manually with the cut tool.
In addition to a gap between members of the same group there is an option for a gap between differing groups. This box will only be editable when the it is potentially applicable. For example the option will always be grayed out when editing "Group1" or the first group of weldments.
The values of intra and inter group members do not have to be equal but the feature manger values will effect all edges in the grouping. If a single joint requires a larger or smaller gap it must be addressed separately. This can be done by clicking the purple dot located at the joint vertex. Once clicked a separate window will appear in the graphics area. Marking the "set corner specific weld gaps" option will allow editing of the gap value field
The methods above work primarily for weldment members created in the same feature. Where a joint is made from members of differing profiles, or otherwise created in different features it is not always possible to control the gap during the member creation. Sometimes when joints leave overlaps or comlicated corners a trim is required to properly model the component. When using the trim tool and option again exists to control the weld gap.
This option is only available when the cut type is a "Simple Cut", when the "Coped" cut option is selected the filed will not appear. To create a gap for a Coped end part there are other options, specifically the "Move Face" tool tend to work (Insert>Face> Move). Other manual cuts will also work to place a gap in the weldment.
These small gap details will surely be a part of any CSWP exam and knowing how to quickly alter each joint and value will help pass the exam. For more review see the main CSWP Exam review post.
To start creating a weldment a path for each member must be present. This means a sketch must be created to represent the members paths. For simple boxes and very basic weldment parts sketches can be laid out in a traditional 2d fashion, but to really control things it is typically easier to create a 3d sketch. With the ability to locate a point anywhere in space, sketching in 3d is sometimes difficult. There are some tricks to help simplify the process.
First to start a 3D sketch select it from the drop down below sketches (seen below) or Insert>3dSketch. Note that because the 3dsketch is a drop down, if you use the toolbar to exit sketches it will take an extra mouse click to get out of a 3dsketch. Instead to when it comes time to exit the sketch
All the same sketch tools will apply for 3dsketching, but how to constrain the points of each entity is key. Initially a triad will appear with two red axis and one black axis. The two red axis are the plane on which you will be sketching. Hit the Tab key and the plane will change.
This allows a rough sketch to be created at first, but even with the two red axis highlighted it is possible to put a point on another plane. When doing so a box will be drawn with yellow build lines. This is only for visual purposes and shows a user where the cursor is in 3d space. All of this becomes a bit confusing, and there are times when even in a 3d sketch it is important to say on the same plane. 3dSketch planes help accomplish this. Similar to reference planes, 3d sketch planes can be inserted for referencing purposes. Right mouse button click while in a 3d sketch and select the "Plane" option (image below).
After selecting this option a feature manager will appear allowing for the creation of a 3dsketch plane (image above). This is NOT a reference plane. 3dsketch planes are contained within a 3d sketch and will not appear as a feature in the feature tree. In the image below three 3dSketch planes have been added but it is clear in the feature tree that only one feature is present, the 3dsketch
You can sketch on the 3dsketch plane by selecting that option from the original sketch drop down icon (3d Sketch on Plane) and then selecting the plane. Once this has occurred the sketch tools will lock onto that plane until another action is taken, no more 3 dimensional dashed yellow build lines.
Dimensinoing is also imporatant for 3d sketches. Nothing is different about dimensioning, the smart dimension tool still works like a charm.
The one thing that may be difficult when dimensioning is figuring out what exactly is being dimensioned. Because an entity is in 3d space it is conceivable that it could be dimensioned in all three as well as a length dimension that spans all three. If a dimension is selected and not placed moving the cursor around may toggle these option. For tight spaces the placement of the dimension may be difficult so lock in which plane the dimension references by clicking the right mouse button.
Another handy option when creating 3d sketches is the ability to put a point on a plane. Ctrl select a point and plane (it can even be a 3d sketch plane) and the add relation option will include an "On Plane" option. This reference does exactly what is expected.
Using all of the above will help to create a clean, fully dimensioned 3d sketch that. With so much power it is possible to create a massively complex weldment structure with only a few features.
3d Sketches are just one of the suggested study topics for the CSWP Weldment exam. To review for other portions of the CSWP Weldment check out the main post.
Edit: Franco Folini of Novedge has addressed this issue with a much more acceptable approach. Now the "read more" opens the article while maintaining a Novedge banner on top. Much like StumbleUpon and other aggregators, comparing the previous Pulse to Reader and other RSS readers (that require a single user to add their own feeds) still seems like a stretch. Just because an RSS is "Public" does not mean you can up and take it. I am satisfied with the resolution as it displays the content along with everything else (3dEngr blogroll, ads, sidebar etc) and makes it clear that the article was not written for Novedge. This post will remain here though my outlook on Novedge has brightened due to the prompt response and resolution.
I have known the Novedge "Pulse" to regularly print synopsis of articles I write for this blog www.3dEngr.com. In the past I thought the extent of their coverage was a small synopsis, and it didn't seem like they were getting much coverage as the incoming visitors from their site were minor blips on my analytics account. Low and behold their is probably a reason for that. Today I realized that entire articles were being reprinted. I found this out when I clicked on a Twitter link (offending Tweet http://twitter.com/_Pulse_/status/9984318337). Not only are they reposting entire articles, they are actively marketing and driving traffic to the reposted article.
I was hoping that this was a one time error. It's not. This seems to be a trend for Novedge. Pulling content and reprinting it. The articles appear next to a picture of me, the picture is ONLY used one place on the internet, that being a Solidworks Forum account. I recently signed up for another of their services, Space Claiming, a forum that centers around the Space Claim product and features Novedge's namely prominently. As soon as I signed up they had already filled in my profile picture with an image that again only appears one place on the web, this time a virtual copy of my personal resume.To their credit, two of the above sources include no form of copyright (the Solidworks Forums may somehow, but my resume has no specific mention).
NOT TO THEIR CREDIT, this blog does include a fun little Copyright tag at the bottom. It should seem both explicitly and implicitly than that reproducing articles is not allowed. They didn't do this just once either, there are 27 blog posts that are blatantly reposted with no omissions at all. Not quoted, just reposted. A complete list of them is under my own name, clicking more gets to the complete post.
Even if it is not explicitly laid out, this seems like a terrible breach of ethics. I also recognize this is not the case for other authors that are picked up in the Pulse section. Some authors only get a synopsis so that a reader who is teased must click the slightly hidden link to get to the original site and read the rest of the article. Others it seems have been stolen from as well (or gave permission) and there is no noticeable pattern.
I'm not sure if this is some sort of shakedown or I am somehow required to "opt out" of novedge to keep them from stealing my content. Either way it is unsettling.
What makes this all so bad is that Noevedge is NOT a news aggregator. They are a storefront. Everyone of the stolen articles appears with an ad next to it. In addition to the add the page also has a few tabs across the top, one clearly being their "Store". Also on the page is a phone number for novedge, call the number and get an automated response "Thank you for calling Novedge, if you know your parties extension please dial it now for SALES PRESS 1". And what do they sell? Training materials, including for Solidworks and CAD Programs including Alibre (which appears often in my own adwords on 3dEngr) and a few others which I have drafts to review as part of the CAD Programs series of posts.
I do not make a living from this blog so I will not claim that they have somehow stolen my livelihood, but by doing this to a variety of content providers they have built a nice collection of useful information which no doubt helps there store. I am not one to stir things up but this sort of shady business practice really irks me. I have requested via the novedge "contact us" form that they correct this issue and only post synopsis of my articles but removing my stolen content is not enough. Novedge is still clearly profiting from stealing content of others and re-purposing it next to their products. There business plan does not appear to include any proprietary products, rather they are just a reseller. Hope business has been good novedge, I'll surely never be purchasing anything from you.
For those skeptics I took a quick screen capture video showing what is happening. Here you can see the list of post they've taken along with the picture. Also visible are there ads. Near the end of the video it shows a post by Deelip and just a summary rather than the whole post.
It is a simple fact that weldments are not going to just be made up of members. Welding can create a strong bond, yes, but there will also be a need for bracing to transfer the loads correctly. To do this many beams get cross braces of smaller sizes or just a simple gusset. When it comes to the basic gusset Solidworks again has a built in option. Insert>Weldment>Gusset or the Gusset icon on the toolbar will both get things started.
Above I have selected two faces, between which I would like a gusset placed. Usually this is two opposing faces to a member, but it is interesting to note here that the gusset feature does NOT require a part to be a weldment part. Gussets can be added even to normal parts that contain no weldment information of features.The criterion for faces is that they can no be coplanar (ie. 180 degree between them) and they must interesect. So again even on non weldment parts a gusset can be used, though ribs will accomplish most of the same tasks and seem to be a better work flow.
There are some dimensional options that can then be specified for each gusset. Length and height are fairly straightforward, as is thickness. The location on the other hand can require a few clicks to get the right orientation. Above is a gusset which has a location of centered. It is clear from the image though that the gusset falls to one side of the center, this is because of the select box of it's thickness.
In this image the thickness is constructed as a mid-plane which properly centers the item. If the driving sketch were turned off, or the gusset was viewed from an angle other than perpendicular it would be easy to make this small mistake. In the case of the CSWP where the center of mass is usually requested a few small errors like this could make a passing grade drop to a failing grade.
One of the other options for the gusset is the internal chamfer. Here is is simple to select the option and reveal the other value boxes in the feature manager.
Of course, not all gussets will necessarily be simple triangles or gusseted. Though those designs tend to be used due to their ease of manufacture some other functions may be preformed. When another function is preformed on a gusset it will change the name of item in the weldment folder manager. If for some reason a cut/extrude/fillet was added the item will no longer carry the Gusset name unless the cut/extrude/fillet is renamed to read "Gusset". This is a minor detail but knowing how names propagate to the folder manager can help to trouble shoot problem parts. (items are always named after the last feature to modify them)
The last thing to note on gussets pretains again to what they fail to do. Gussets on some members will extend on the outside of a joint and cover an entire joint. This can be seen on bridges or large trusses. Rivets are used to attach the gusset and by putting them on the outside of all members the load can be distributed more evenly on the member. These types of gussets can not be created with a gusset feature. In the above image I have tried to select two faces to show this and clearly the option fails. There are a few workarounds to this, a user can create an outside oriented gusset and extrude/move the faces as needed. Or to simplify the process a manual gusset can be designed. simple extrude a new feature off of one of the faces in the profile required. If the part is already a weldment this new extrude by default will create a new body, then simply rename the extrude feature to say "gusset" and due to the naming system it will appear in the cut sheet as such.
This is just a basic overview of the gusset feature. More reviews on other weldment items can be found through the CSWP Weldment review post.
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.
Alibre Design
When looking at getting new CAD software it is a simple fact that one of the key criterion when making the final decision is price. Alibre identified this and has recently made some news by dropping the price on their basic software package to an affordable $97. They tout this on their website very clearly:
Alibre Inc. offers the industry's most affordable complete engineering solutions. Founded in 1997, Alibre Inc. is led by visionaries who sought to change the landscape of 3D mechanical CAD/CAM software by providing full parametric CAD technology to anyone that needs it, versus only to those in the relatively unique financial position to afford traditional CAD systems.
... Beginning with ComputerVision in the 70's, the price for the technology started at around $1,000,000. Catia in the 80's realized a $100,000 price tag. Pro/E at the end of the 80's saw a $20,000 price tag. Solidworks continues the trend in the 90's with $5000 per seat costs. And Alibre comes in to deliver the same technology starting at $97. The era of exclusivity for advanced design software is over.
The reference to the "90's" pricing of a software means the marketing copy may need some updating, but still the numbers are fairly close to the current going rate. The jump from 5 large to sub $100 is Alibre's attempt to bring 3D Cad main stream individual and home user.
Maybe because of the recession and a nationwide shrinking in spending there has lately been a resurgence of DIYers. The DIY trend has spawned an entire industry. Popular blogs and magazines such as MAKE and Instructables get thousands of hits. TV shows got in on the trend with How It's Made, Myth Busters, and to some extent Extreme Makeover Home Edition. There are even subscription based machine shops opening around the country (Techshop). By dropping their price under $100 Alibre is taking their shot at this expanding market which means a business model of low price, high quantity.
So what does this low price get you? Is the desire to cater to a larger audience detrimental in any way? The Alibre software is available for a 30 Day free trial (another good marketing tactic), and I signed up to take it for a spin.
Installing Alibre and System Requirements
Alibre is availble as a download for install. The trial version (which is a 30 day licesne of the $497 design Professional) took all of maybe 25 minutes to get. Everything installed in a few simple clicks. They sent the registration information to my email and it is worth noting that the 30-Day time period did not begin until the software was opened this information put in. This was nice since I had about a 5 day lapse between signing up and downloading and getting the chance to actually poke around.
Windows XP, Vista or Windows 7 (32 or 64Bit)
IE 6.0 or higher
.NET framework
J# Redistributable
Microsoft DirectX 9.0c or higher
2GHz Intel Pentium or equivelent
2GB Ram
1024x768 screen resolution
64MB Video Card supporting DirectX 9.0c
500MB disk space
Tutorials and Learning Alibre Design Software
YAY! I can rotate in three dimensions with using a keyboard. Right+Left Simultaneous allows for spinning, middle mouse click and hold moves the object and scrolling zooms. RMB even brings up an in context menu. With some knowledge of CAD already it is easy to tell what each portion of the software is going to do, and hovering over the buttons further clarifies with the title. Sketching is still the basis of parametric CAD tools and Alibre is simple to figure out in this regard. Assemblies and Motion are more detailed and typically require some documentation.
There are built in tutorials for Alibre, as well as an online library of simple features. Although these seem to cover a wide range of topics it only really scratches the surface. Each tutorial is comprehensive in it's own right and will allow a user to utilize each tool, but they are lacking overall. The material itself is extremely verbose, the layout of the tutorial is rather poor, and although models are reused the seemingly random and disjointed nature of the tutorials is frustrating. This is not a knock on Alibre, as most CAD systems seem to have neglected the built in training. It is my suspicion that this is a business decision thanks to the VAR distributer method of most programs where resellers really make money training users.
The smaller user base means that my usual resources (Google searches and Youtube) turn up a fraction of the information of other systems. The most complete and easily named play list on Youtube only covers drawings:
Not a big deal in the grand scheme of things but for new users who like the hand holding walk through this may be a downside.
First Model
Although there are 30 days on the trial there is simply no reason for me to really delve to deeply into this software. The functionality is fantastic for the price but with access to other systems (my bread and butter) dealing with a different mouse click and workflow is causing me issues in the daily routine. Before signing off Alibre though I took a shot at model just a basic vessel. Nothing ground breaking here, just a few quick extrudes, a shell and some sketching.
The drawing was also fairly easy to pump out, and of course with a parametric system updates to the model propogated to the drawing.
File formats are worth noting. Solid Model files are saved in a proprietary format for Alibre but they can also be exported to Iges and Step. Drawings again save in a proprietary format but also can be exported to .dwg, .jpg or of course printed to .pdf.
Overview
Really if it comes down to price there are few if any other options that compare. To my knowledge there are no free options that create quality manufacturing drawings, and Alibre delivers on that for as close to free as it comes. The pricing structure does make a jump though, from $97 to $499 . Learning the software is relatively easy and users with experience will find the standard tools easily, though the minor details (click-hold>drag vs. click>drag) can be cumbersome at first. For companies with basic designs and no desire for flashy renderings, where documentation is required and cost is always a concern Alibre fits right in. Hobbyists and DIYers looking for a cheap, functional solution also should check it out. The 30-day trial is always free and if it doesn't work out there is surely no harm.
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 CAD Programs tab.
Sweet Home 3D
It always surprises me the places 3D is still NOT used and Sweet Home 3D is one of the reasons why. Included in the software are loads of common items that can be dragged and dropped into a scene. The ease of the tool, and the simplicity of it's functions are why I start to wonder why someone like IKEA or Home Depot hasn't bought the software. Hire a couple CAD jockeys to model a complete catalog of furniture and immediately you have a tool that will let people dream up all sorts of purchases.
Sweet Home 3D is dead simple and the learning curve on it is minimal. A few tweeks to the graphics of each button and even a monkey could figure it out. The User Guide is a great tutorial and because of the nature of the program it is really all the documentation that is needed and if it needed to be condensed it's possible to get the primary functions down to a few paragraphs. Models can be added to the library so long as they are in OBJ, LWS or 3DS format which are easy enough to get using most major CAD programs along with a sampling of free tools to help (Meshlab, Blender both will take in and save out various files).
The graphics leave something to be desired but it is easy to kill off an hour or two using the browser version, just dragging and dropping random items into the scene. If you have an image file of a floor plan it can even be imported to help with the layout. The video below is straight from the user SweetHome3d on Youtube and shows a little about what can be done.
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. 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.
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. Above 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.
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. 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.
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