North America's Leading Siemens PLM Partner
To understand how this works, let’s fist look at an ordered part. Below is a sketch for a part that I wish to model. Notice that I have fully constrained the sketch.
The sketch has zero degrees of freedom, so I can predict what will happen when I make a dimensional change to any of the 3 values. I control part of the sketch with geometric constraints, which include the following 2D relationships:
When I use the sketch to create a model, the sketch becomes the parent of the solid model, as shown below:
I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.
Now let’s make the same part in the synchronous mode. We start by making a sketch, as shown below:
Notice that I can fully constrain the sketch in synchronous mode. The difference here is that when I create the solid, only the dimensions are migrated to the 3D model. The 2D geometry and 2D geometric constraints are left in the Used Sketch header on the PathFinder. In other words, no parent child relationship is created between the sketch and solid, and the 2D dimensions are converted to 3D driving dimensions on the model, shown below:
Notice that 3 of the 4 dimensions are red in colour, while the depth dimension is blue. A red colour means that the dimension is locked and can only be modified by a direct edit of that dimension. Let’s make the fourth dimension locked as well.
So now we have the dimensions fully constrained or locked. What about the geometric constraints? Since the 2D geometric relationships have not been transferred to the model, a lot of users become concerned that the model is no longer fully constrained. They are partially correct. Let’s take a closer look at the model.
By the nature of the solid, we can make a few assumptions.
1. The connect relationships will be maintained at the model level. Why? Because if they are not we no longer have a solid.
2. Synchronous edits use Live Rules, and Live Rules will maintain most of the pre-existing geometric situations. For example, if you attempt to change the values in the part, default Live Rules will keep the walls in their current horizontal/vertical position.
3. Synchronous will only analyze the effected faces in any move. Therefore it only has to re-compute faces affected by an edit.
Even with these assumptions, there admittedly could be some un-expected results if you are using this model in a custom program or configurator. So how do we eliminate potential un-expected results? We use 3D geometric relationships.
Persistent (3D) relationships
Looking at the original sketch of our model, you’ll notice that the sketch was centered on the base coordinate system. I can do the same with the model by using the horizontal/vertical persistent relationship command. I’ve placed these relationships in the model, shown below. Notice that they also are listed under a Relationship header in the PathFinder.
I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.
For more complex models, synchronous offers even more 3D geometric relationships.
Some will argue the fact, but the truth is the majority of ordered models that I see from customers are under-constrained. Because of the parent child nature of ordered modelling, this could be, and often is a problem when editing ordered part models. If you doubt this statement, go back to your database and open some of your existing models. Under the Solid Edge options > General tab, turn on the ‘Indicate under-constrained profiles in PathFinder.
If a red pencil icon appears anywhere in the PathFinder, you have under-constrained features.
If you would like more information on synchronous technology or would like to attend one of our synchronous training sessions, please contact us at [email protected] or visit our training web page at http://www.designfusion.ca//technical-training.html.
Last year at Solid Edge University (SEU2013) I was introduced to CAMWorks from Geometric. What I had always considered a competitive product was now being offered as an add-on to Solid Edge. Being a long time NX CAM user, I was a little surprised that Solid Edge would partner with another CAM package, especially one so closely linked to another CAD package. At my company’s request, I put aside my skepticism and started to find out what I could about this new offering.
The first release of CAMWorks for Solid Edge was limited to 2.5 and 3 Axis Milling and Turning. Since most CAM packages can easily handle this type of manufacturing, I focused on what made CAMWorks unique, and how it worked with Solid Edge. Three distinct factors stood out for me during my initial analysis of the product:
1. CAMWorks for Solid Edge is embedded and fully integrated into Solid Edge.
When you install CAMWorks for Solid Edge, it becomes part of Solid Edge. A CAMWorks ribbon is created, and a CAMWorks edge bar is added to the PathFinder.
This eliminates wasted time and potential errors in loading your Solid Edge model into external CAM packages. Plus you can easily switch back and forth between the CAD and CAM ribbons, to make associative edits or revisions.
2. CAMWorks for Solid Edge utilizes feature-based machining to allow for rapid tool path generation.
CAMWorks for Solid edge utilizes automatic feature recognition and an advanced database to create some truly impressive knowledge based machining. Once setup the basic workflow is as follows:
- Identify the parts for machining
- Extract features to be machined
- Generate the Operation Plan (utilize the database to determine how the features are to be machined)
- Simulate/Verify the toolpath
- Post process to create the G-code
If the database is setup correctly, each process is automatic. I’ve seen situations where you can go from CAD model to G-code in 5 button clicks, if you skip the simulation step.
The database (TechDB) used in CAMWorks for Solid Edge, can be set up differently for each company and even each user. This allows companies to capture and reuse their best machining practices, saving time and eliminating repetition. It should be noted that you can create operations on the fly and save them to the database, allowing you to continually expand and improve your knowledge base for future machining. The potential exists to reduce programming time from hours to minutes, but it does require some up front effort to realize this kind of result.
Despite these impressive points, I wanted to learn more about future plans for the product. Two weeks ago, I was invited, by Geometric, to attend a training session for VAR’s in Scottsdale, Arizona. I eagerly accepted the invitation, mainly to escape the brutal winter we’ve been having, but it also gave me an opportunity to get answers right from the source.
I was not disappointed; the temperature ranged between a balmy 25-28 degrees Celsius, and the capabilities of CAMWorks exceeded my initial expectations. They have recently added Multi-Axis milling, Mill-Turn, and Wire EDM capabilities and continue to work with Solid Edge to improve the product.
As a combined result of my investigation, and the work of our management team, we will be adding CAMWorks for Solid Edge to our product line. We believe this will complement our existing products, and provide more choice to our customers. We will be adding more information to our website, as it becomes available, and have plans to offer training in the future. In the meantime, if you’d like to learn more about CAMWorks for Solid Edge, please contact your account manager or contact us directly at [email protected].
When I had landed, a thought came to me; and that was that I have never seen a turbine engine airfoil blade or wing model in Solid Edge. So I took it upon myself to do some research on how I would model airfoils. I came across some interesting web sites that explain the whole explicit mathematical functions used for 2D curve definition for airfoil design; very fascinating however, I just wanted the basics.
Here is the basic anatomy of a blade; you have root type, root width, root height, and airfoil height.
For many years, research and studies have been conducted on airfoil blades and also on the performance of wing design aerodynamics. Shown below is an airfoil generator for blades that I found online.
As you can see by entering the appropriate values you should be able to generate an airfoil based on you requirements.
Geometry Airfoil Generator Example:
After generating the foil you have two options, either to create a DAT file or simply copy and paste the X,Y,Z coordinates to your excel.
I chose to just simply copy and paste directly to Excel. Notice A=X B=Y C=Z, in some cases if you are creating a simple airfoil you may only get XZ coordinate values. If that is the case you need to insert a cell and enter zero for Y as shown in this case.
1. Before you start anything you will need to model up the root type, make this part in ordered. Surface modeling works best on the ordered mode. I downloaded a CAD model from GrabCAD website. If you have the time to model, a basic shape like shown below, make sure the XYZ origin is setup correctly. Therefore, when creating the airfoil via the Solid Edge curve by table option, it is placed correctly on the root top surface.
2. Next click on the curve by table option. It is located in the surfacing tab on the curves group.
3. Click on browse, then find the excel files.
4. Select finish. Notice the 2D airfoil automatically sets on the origin.
5. By clicking on the edit points data step, the Excel sheet will open. If there should be a need to modify the XYZ points manually you will be able to do so at this step. Click finish when you are satisfied.
6. Another option is to set the curve fit and curve end conditions.
7. On the next step, we are going to create two User coordinates systems.
Under the surface tab, find coordinates system on the planes group. This will allow us to place new airfoils at any point in space.
Select (key-in (relative to another Coordinates system)
8. Enter 3 on the (Y), next then preview and then finish. Repeat the same step for the second UCS, except enter 6 for (Y).
You model should look like this.
Now, we can continue since we have created the UCS to place the airfoils.
9. Repeat the same steps for the second airfoil. You may have as many airfoils as you wish- usually that varies on how
complex your blade may be. For this example, I will only be using three airfoils.
10. This time before clicking on finish, select the second coordinate system (the names may vary).
Repeat for last Airfoil.
Your model should look like this: Root with all three USC in place.
11. We are now going to create a BueSurf. This will create the outer shell for each airfoil, thus creating the turbine blade.
12. Click on the BlueSurf command, located on the surfaces group.
13. Select the first airfoil sketch.
Make sure the cross section vectors are consistent with the other geometery.
14. Select on the second airfoil sketch, notice again the vectors are consistent with the first selection.
15. You model should look like this.
16. Continue on with the selection
The overall blade has been constructed, we will now add rotation to the blade. Some blades have more complex geometry, I’m only using three airfoils to crreate a simple blade
17. Select the origin, and then click on edit definition.
18. Click on the orientation step.
19. Enter 25˚ for the Y direction.
Notice the foil is now 25˚ about the Y
20. Repeat the same step for the last coordinate system. Enter 30˚
21. You have completed this turbine blade using a geometry generator with BlueSurf. I hope you enjoyed it.
Did you know that you can do this in Solid Edge . . .
As a support team member, and technical trainer, part of my job is to learn the technology inside Solid Edge. Therefore, I’m allotted time to learn, test and research the latest technology. But as I’m sure many of you will agree, this is a privilege most users don’t have. Users are under the gun to meet deadlines and therefore often stick to what they know, even if it’s not the most efficient approach. As a result many users are unaware of the full potential of Solid Edge.
On more than one occasion I have received requests for custom programming for capabilities that already exist in Solid Edge. I often find myself saying “Did you know that you can do this in Solid Edge already”. With this in mind I thought it might be a good idea to start recording some of these moments and share them in our blog. So below are some of the questions I get from our customers along with how to do it in Solid Edge.
I have to delete a part list from my draft file, is there a quick way to delete all my balloons, or do I have to pick them individually?
Did you know that you can do this in Solid Edge using the SmartSelect command? To select all the balloons at once do the following steps.
- Pick the Select tool to launch the Select tool command bar.
These are actual questions that I have received many times from our user base. It just goes to illustrate that Solid Edge is not always being used to its full potential and that there is always room for improvement. The more you understand about the software the more efficient you will become. I plan to continue sharing the more popular questions, from our tech line, in future blogs. If you are a customer of Designfusion’s, and have a question, please don’t hesitate to call our tech line at 1-877-215-1883 or email us at [email protected].
Siemens PLM Software has announced that this year’s Solid Edge University will be held in Atlanta, Georgia on May 12-14, 2014. For those of you who have not attended this conference, you are truly missing a great opportunity. Not only do you get a preview of the next release of Solid Edge, but you get to connect with the Solid Edge developers and provide input to the direction of future development. You can also participate in hands-on learning, attend presentations given by CAD users and meet with experts from all aspects of the design continuum. Focus areas will include CAD, design data management, simulation, manufacturing and a host of complementary applications to help you design better. Some of us at Designfusion will be presenting again at this year’s conference.
This is also a great opportunity to visit with our sponsors and technology partners and learn new ways to enhance the power of Solid Edge. Many partners are set up at the conference, ready to answer any questions you may have. Plus there is no better place to network with other Solid Edge users who make up this vibrant user community. I personally spoke with the Designfusion customers who attended last year event and everyone said that the learning experience was well worth the cost of the conference.
I hope you can join me and my colleagues at the Solid Edge University 2014. For more information, and to take advantage of the early bird registration, go to the Solid Edge University website at http://www.solidedgeu.com/.
In the past few days, customers have called about revision manager and have asked several questions on how they can move or copy assemblies to new locations.
There were a few main issues custumers have had in regards to Revision Manager, and what I have done is created multiple scenarios to tackle these issues .
Scenario 1: Copy all assemly with all parts to new location.
Scenario 2: Copy all parts associated to assembly and folder structure to new location folder.
Scenario 3: If a folder with parts related to an assembly gets nenamed and links get broken, how to redifine links.
Sample Folder structure (this can be any combination of folder locations) the point is that, we need to move or copy files to a new location.
Scenerio 1: copy all assembly with all parts to new location, this is ideal when you need to clone
the whole asssembly to send to a customer.
5. Final step is to perform actions. At this point the assembly is copied to the (new) folder location.
Scenerio 2: Move the whole assembly with subfolder structure and related files only.
Another method is just to copy all folders to the new location, but note that there may be
files that do not relate to the assembly.
In cases where you only need to move files that relate to that top level assembly and keep the
same folder structure, files not related will not copy or move.
6. Open selected assembly with revision manager.
7. We are going to move to (new location) and copy the same folder structure. By selecting the (rename)
you are moving the files from the (original) folder.
8. Notice action is to rename document.
9. Now click on replace old folder (Original) with new folder (New). Then select replace all then cancel.
10.Once replaced, see new folder with new location.
11.Click on Yes and close Revision Manger.
12.Notice the new folder structure in new location, notice the subfolders are copied as well.
13.Review new folders using window explorer to take a look at the previous folder location; notice only
files that were not associated to the assembly did not copy (This is also a good way to isolate
assemblies) with the folder structure. This complete this scenerio.
Scenario 3: Cases when a folder gets renamed and then you open the assembly and notice that
all links are broken. This is very common in networks with many users.
14.So let’s go ahead and rename each folder as shown below, just by adding “1” at the end of each
If you try to open the assembly now with RM or Solid Edge, the files will not open; you will get a notice
that files are missing.
15.Click on the redefine links then select top level folder then ADD (make sure that the subfolder is
16.The easiest way to get the folder address correctly is by going to the window explorer, and then copy and paste.
-(ManufacturedParts) is the original folder
-(ManufacturedParts1) is renamed folder
-click next twice
17. Click on Back twice
18. Repeat for other folders
This was also presented at one of our Solid Edge Productivity summits by Barry
To learn about the other settings, click on the Help button. The help documents have a complete breakdown of all the other settings.
In the image above you can see that after I selected the part file and I am given a Front view of the part, attached to my cursor, along with a command bar. In this example I am using the horizontal command bar. I could also use the vertical command bar as shown in the following image.
I can place this view on my draft sheet and I am immediately put into the principal view command. This allows me to place alternate companion views based on the position of my cursor. For example, if I want a Top and Right view, along with the Front view, I simply move my cursor up and click for the Top view.
I can then move my cursor to the right and click for the Right view.
To exit the command I hit the Esc key, on the keyboard.
As you can see there are over a dozen options here. I will focus on the 6 most common, but a description of all the options can be found in the Solid Edge Help section.
• For Part or Sheet metal files.
• For an Assembly file.
This option allows you to select additional views to place along with the primary view. You also can change the orientation of the primary view. When you select it the following dialog appears:
This option allows you to change the view orientation before you place it. For example, if you just wish to place a single view, you can control the orientation by selecting this option and choosing from the following drop down list:
Best Fit, Set View Scale, Scale List and Scale value
2. Set the Flat pattern option.
3. Select the scale that I want to use. But do not click to place the view yet.
5. Place your view.
Following the same steps I could save another layout showing the Front, Top, and Right view for the same model, and save it as “FTR_view”. The next time I run the Drawing View Wizard on a Sheet Metal part, I could select from either layout.
Note: I find saving layouts easier if you always start with a new draft file, per layout.
• Items stored in the saved settings: