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Did you know that you can do this in Solid Edge . . .

John Pearson - Tuesday, February 11, 2014

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.

 

   

            

  • - Select the SmartSelect icon from the Select tool command bar.

 

 

  • - Select one of the balloons from your view.

  • - The SmartSelect Options dialog box appears.  Check Element type and click OK.

 

 

 

 

 

  1. - Notice that all the balloons highlight.
  2. - Hit the Delete key and they are all deleted.
  3. The SmartSelect command searches the active sheet for other elements with similar attributes, such as element type, color or line width. All matching elements are automatically added to the selection set. Now you can make changes to the selected elements all at once. This is ideal to make changes or delete dimensions, lines, callouts, etc. in the Draft environment.
  4. I have a large assembly and when I’m zoomed in and try to rotate the part, it flies off the screen. Is there a better way to control the rotation? 
  5. Did you know that you can do this in Solid Edge using the middle mouse button? The problem here is that the default center of rotation is (0,0,0). So if you are zoomed in, away from the origin, any rotation appears to rotate out of view. What you need to do is change the center of rotation by following these steps:
  6. - Zoom into the area you want to view.
  7.  
  8.  

     

  9. - Click your Select tool. Notice that the cursor has a small gold box beside it.
  10. - Click the middle mouse button, in an empty space, and the gold box will disappear.
  11. - When the gold box disappears, move the cursor over the model. Notice the bright pink dot attached to the cursor.
  12. - This bright pink dot represents the center of your next rotation. Move it to where you want the center of rotation to be, and then hold down your middle mouse button to rotate.

 

 

  1.  
  2. - Notice the rotation symbol on the cursor, and that you are rotating around the pink dot.

 

  1. When you release the middle mouse button you are placed back into selection mode. You can also use this in the part or sheet metal environments. For more information, and additional mouse tips, read the Solid Edge Help docs under the “Using the mouse” heading.
  2.  
  3. I want to place a dimension between two points that are not horizontally or vertically aligned.
  4. Did you know that you can do this in Solid Edge using the Distance Between command? All you have to do is follow these few steps:
  5. - Select the Distance Between command.
  6.  
  7. - On the command bar, change the Horizontal/Vertical option to By 2 Points
  8.  
  9. - Select the 2 keypoints and place the dimension.
  10. For more information, and additional options, read the Solid Edge Help docs under the “Dimensioning overview” heading.

 

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 support@designfusion.com.

  • Using the Improved Drawing View Wizard in ST6

    John Pearson - Thursday, December 26, 2013
    As more and more users migrate to Solid Edge ST6, I am receiving more calls asking about the Drawing View Wizard. There was a major overhaul in ST6, but do not panic, for you can reset it to behave as it did in previous versions. The new method utilizes the toolbar approach which is found in most Solid Edge commands, where the old way uses the wizard approach.

    How to set the drawing view command to the wizard method

    A new tab has been added to the Solid Edge options in the Draft environment. The tab is entitled Drawing View Wizard, and allows you to define some default settings.

     


     

    To learn about the other settings, click on the Help button. The help documents have a complete breakdown of all the other settings.

    Using the new Drawing View Wizard method

    If you leave the previously mentioned option checked, you will use the new simplified workflow for placing a drawing view. The simplified mode reduces the number of steps required to generate drawing views. It omits the wizard dialog boxes and instead displays the View Wizard command bar at the drawing view placement step. This is the default mode for the View Wizard command.


     

    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.

    Note: You can choose whether you want to use vertical or horizontal command bars in the Solid Edge options, under the Helpers tab.

     


     

    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.

    Preselecting layouts and presetting options

    Before I place any views I can preselect layouts or preset some options. All these options are on the command bar. The image below is that of the vertical command bar. I use this for training because it shows the option names.


     

    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.



    Drawing View Wizard Options   

    This option allows you to specify content and display options based on whether the drawing view is an assembly, part, or a sheet metal model. When you select it the following dialog appears:


    •    For Part or Sheet metal files.

     

     


    •    For an Assembly file.

     

     


    For those of you familiar with the old Drawing View Wizard, you will recognize these dialogs as the first dialogs that appear. All the options that you are used to are still here.

    Drawing View Layout  

    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:

     

     


    Once again this dialog should be familiar to existing Solid Edge users. It is a combination of the 2nd and 3rd dialogs of the old Drawing View Wizard. Here you pick your primary view and the companion views. Note that the primary view can be a preset view or a custom view.

    View Orientation

    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:

     

     


    You can use this option if you don’t plan to add companion views.

    Best Fit, Set View Scale, Scale List and Scale value

     

     


    These options allow you to control the size of the view that you are placing. They are identcal options that you would find in the previous Drawing View Wizard command, and are used the same way.

    Saved Settings

    This is a new and very useful option to ST6. It allows you to save your layouts for reuse in other draft files. For example, if I always place a flat pattern of my sheet metal parts, I can place my first layout and save it. To do this I do the following steps:

    1.    Start the Drawing View Wizard command and select the file that I want to place onto the draft sheet

     

     

     

    2.    Set the Flat pattern option.

     

     

     

    3.    Select the scale that I want to use. But do not click to place the view yet.

     

     


    4.    In the Saved Settings dialog I name this layout as Flat and hit the save icon.

     

     

     

    5.    Place your view.

     

     


    The next time I run the Drawing View Wizard, with a Sheet Metal part that contains a flat pattern, I just have to select “Flat” from my saved settings.

     

     

     

    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.
    There are a couple of things to note here.
    •    To use a saved setting, that setting has to be selected before the drawing view is placed on the drawing sheet.

    •    Your saved settings are based on model type and model size. For example if I place a part file, I will not see the Flat or FTR_view saved setting, because I created them using a Sheet metal part.

    •    Your saved settings can be predefined per model type and model size (for assemblies) on the Drawing View Wizard tab (Solid Edge Options dialog box).

     

     

     

        Items stored in the saved settings:
    o    All properties from the properties tab.
    o    View orientations
    o    Custom orientations
    o    Best Fit
    o    Set View Scale
    o    Shading Options
    o    Edge Colors

    •    Saved Settings file will be created in the reports directory called DraftWizard.txt.

    Once you’ve created a list of saved settings, I believe that you’ll find the new approach more efficient and easier to use. But if you still prefer the old method, you can still use it. As always, if you have any questions, and are a customer of ours, please call us on the toll free tech line at 1-877-215-1883 or email us at support@designfusion.com. If you are not a customer of ours, please contact your reseller for further support.

    How to create an adjustable coil spring in synchronous

    Manny Marquez - Wednesday, October 30, 2013
    In the September 18th  blog, we showed you how to create an adjustable coil spring using the Ordered/History modeling techniques. We can take different approches as to how to model this spring. We can use helix or wrap sketch techniques, but that doesn’t mean we can make the spring adjust using ST. In the following steps, we will take a look at how to model the coil spring using  ST modeling.

    1. Create all sketches as needed. We will start with sketching path for all features.



    2. Select sweep. We are going to use the Twist option


    3. At this point the twist option is not selectable.



    4. Select the path then accept.


    5. Then pick on the cross section.


    6. After selecting the cross section, you will get this message. It’s Ok, just click on EDIT, and then edit definition.


    7. Notice that the Twist option is now available. For the first feature select number of turns of (-1.0)


    8. This is the result.


    9. Next, repeat the same step for the opposite side, using (1.0) for the number of turns.


    10. Click on sweep protrusion.


    11. We will now create the extended protrusion out from the twist using a single path.  Select options as shown click ok. Then select path and accept.


    12. At this point select the cross section.

    13. Repeat step for opposite side.

    14. The next step is to create a revolve protrusion about an axis; we need to draw a line offset from the center of circle. Lock plane then (ctrl+H) this will allow viewing normal to surface


    15. Draw a line .032 from the center of the circle and add a perpendicular relationship from the 33˚ line.


    16. Select the end surface; then drag the steering wheel to the line created from the last step. Snap into the line so the torus is perpendicular to the line.


    17. By selecting the torus then selecting the (lift) option on the ribbon, this will allow the surface to rotate about the center line. Enter 70˚ or appropriate value.

    18.  In this step there are two options. (I used option 2)
    1. Click on the protrusion command select surface as indicated, enter value.
    2. Select the surface as shown, use the lift option and drag .300 distances.

    19. Mirror features for opposite side.



    20. This portion is a very crucial step in order to make this Synchronous part coil deform   
     as the part adjusts.

    I’m going to show you two options to adjust the coil spring.

    OPTION 1
    Select every surface/ feature, except the two as indicated with red arrows; drag the steering wheel to the coordinate system. The torus must be parallel to the direction in which to rotate the part. (See image)
                     (Do not include any of the sketches to rotate along with the part.)

    21.  Select the steering wheel torus, then dynamically rotate the part or enter a value.
       (Notice the two surfaces that were not selected stay stationary.)
    You can repeat these steps at any time if you wish to adjust the coil.

    Remember what value you use. This will be helpful, if you need to change it back to original state.

    FYI:   If you decide to finish the model, then try to rotate to adjust coil spring angle,   this will not work. ST will not allow you to dynamically drag angle from both ends, only   one at either end.

    OPTION 2

    22.  Select the circle command and lock to Base plane to create a circular cutout.
      (ctrl+H)

    The idea behind this is to have live rules recognize the concentric cutout; this will    prevent the coil from moving about the center when we later add an angular   dimension.

    (The Diameter size should be minimum size possible as long as it cuts into coil without making an impact on your design intent.)


    23.  Select the symmetric extrude and remove options from the smart ribbon bar.
     (You can use the space bar to toggle between add or remove)

    24. Add an angle between dimension, select the (y) axis vector from the (UCS) then place dimension.   ( See images)

    25.  At this point select all surfaces except two as indicated with red arrows.
    RMB click to create a user-defined set.

    26. The next step is to select the (a) user-defined set. 
    Then click on (b) angular dimension to start modifying the angle.

    27. As you can see, by dynamically changing the value, the coil is changing and adjusting. Notice the center cutout stays concentric to the center of the UCS origin. That was the only reason to create that cut out, so that live rules recognizes this predictable behavior.

    You can repeat these steps at any time if you wish to adjust the coil.
    Remember what value you use. This will be helpful, if you need to change back to original state

    28. You will create the last feature using the sweep command.



    Select path then cross section.

            (This feature will not rotate or adjust like previous modification.)


      Results



    Note: 
    For future modifications you may need to restore sketches, to use when deleting the feature to reuse after modification is made. In other words, if you need to change the angle, you have to: 
       a. Delete feature.
       b. Restore sketch.
       c. Rotate, modified angle.
       d. Add feature again.

    29. Fence select all parts (except sketches), hit (Ctrl +R). This will allow viewing from right view.

    30. Drag steering wheel to coordinate, snap so that torus is parallel to rotating angle.
    Dynamically rotate or enter a value.

    31. Keep in mind, if you need to modify like in step 19 or 21, delete feature.









    Ordered vs. Synchronous – Which should I use? – Part 1

    John Pearson - Thursday, October 10, 2013
    1. I’ve been approached by many Solid Edge users who ask me if they should be using the synchronous or the ordered method for the designs. I always answer yes. To which they smile and usually ask “No, really, which is better?” To which I respond, why choose? Use both. This may seem like a political answer, but it’s not. The true power behind Solid Edge is the hybrid approach utilized through integrated modeling. To understand the benefits, we first have to look at the pros and cons of each paradigm.


    Pros and Cons of the ordered paradigm


    Ordered modeling has been in Solid Edge since day one. It is like an old friend that many long time users are comfortable with, and experienced in. Many of the users I talk to claim that they like the control that ordered modeling gives them. Ordered modeling forces the user to build the model in a certain order of steps, which are predefined by the intent of the designer.

    For example, the designer starts with the sketch or profile for his/her base feature. He/she draws the profile and constrains it with 2D geometric and dimensional constraints. By doing this he/she is controlling how the sketch can change. This involves some thinking ahead and predictions of potential future edits. 

    Once the sketch is complete, it becomes the parent of the base feature. In other words the sketch drives the base feature. Additional profile base features are then added to the base feature in a similar manner. Each becoming a child of the base feature, thus creating an ordered structure that is shown in the Pathfinder. Treatment features are then added, creating more parent child relationships, until you have a completed model.

    The ordered structure appeals to a lot of designers. Especially, if the design lends itself to a master model approach, where you create a master model and then generate many variations off that model by simply changing a few parameters. This does require intelligent set up of the master model and a good understanding of how the model was constructed.


    So when I ask my customers what they like most about ordered? I get the following list of Pros:

    Very structured approach to modeling.
    Predictability to the designer who created the model.
    Ability to lock down how the model behaves.
    Other users can’t accidentally change my design.
    Easy to set up family of parts or family of assemblies with a master model approach.
    Long accepted method of modeling with a proven track record.  
    Creating the initial model is just as fast in ordered as it is in synchronous method.
    I am use to ordered design and have lots of ordered legacy data.

    From a designer’s point of view, all these are good reasons to stay in the ordered paradigm. However when I look at the list, I get a feeling of déjà vu. It looks very similar to the list of reasons that designers use to give for staying in 2D. But we all know that many companies have switched to 3D. Why? Because the industry recognized that switching to 3D design provided many advantages. In other words there were a lot of Cons in 2D design. So what are the Cons of the ordered method?

    It should be noted that some of the Cons or disadvantages that I am about to list come from working with the synchronous technology for almost 6 years now. Many designers will disagree with some of these because they do not have a true understanding of how synchronous modeling works. So with that in mind let me list some of the main problems with ordered designs.

    Forced structured approach to modeling.
    Modeling requires the designer to predict how the model could change in the future.
    Editing the model is slow and cumbersome if the designer incorrectly predicted the

            future changes, or uses the part as a reference part to initiate a new model.
    Making changes requires an in-depth understanding of how model was originally  

            created.In some situations it has proven faster to re-model the part then to try

            and understand all the parent-child relationships.
    On large models, re-compute times can be lengthy due to the structured approach.
    Models are heavy because of all the history saved in the part files. This makes opening and saving times lengthy.
    Working with foreign data can be a challenge without the history/feature tree.

    I’m sure my colleagues, could list a few others, but I think that these are the main ones. The next question then becomes how can synchronous eliminate or minimize the problems we face in ordered, and is it enough of an improvement to start using synchronous modeling? To answer this question, let’s look at the Pros and Cons of the synchronous paradigm.

     


    Pros and Cons of the Synchronous paradigm


    If you believe the marketing from Siemens, they claim the following:

    “Synchronous technology provides the first history-free, feature-based modeling technology that enables up to 100 times faster design experience.”


    Let me clarify this statement. It is not saying that all your designs can be done 100 times faster. In fact, if you start a design from scratch, the initial design process may only be slightly faster in the synchronous paradigm. However, there are aspects of the design process, which are up to 100 times faster if not more. Synchronous takes advantage of today’s powerful computer processers, and the elimination of Parent-Child relationships, to allow fast flexible modeling. Yet, with tools such as Live Rules, Procedural Features, 3D driving dimensions (PMI), it still provides the designer with control over the design when needed. So let me give you my list of synchronous Pros:

    Rapid, flexible design tools.
    The designer does not have to predict how the model will change in the future. 
    History free approach allows for instantaneous model changes while editing the model.
    The sketch does not drive the model. The dimensions are migrated to the model and directly drive the model at the 3D level.
    Rapid edit tools and handles allow the designer to edit the model without having to understand how it was originally modeled.
    Can edit a part file or group of parts from the assembly level, without having to edit into each part.
    Can edit models from any CAD system as easily as editing solid edge models.
    Model can be constrained at the 3D level, but not really necessary.
    Models are lighter therefore open and save faster than in the ordered paradigm.
    Can convert legacy ordered models into synchronous models.  
    Although a different approach to modeling, it shares many similarities with the ordered paradigm. Thus easier to learn for existing Solid Edge users. 

    Given all the Pros, you may be asking why everyone hasn’t changed to synchronous modeling. I believe that there are a few reasons for the hesitance to change. The first is the way Siemens introduced synchronous technology. It was first launched in the fall of 2007 in Solid Edge ST. It was new, and limited to part modeling with no real tie in to the ordered parts. Many users tried it then, but were left unsatisfied due to the limitations. The following year Solid Edge ST2 was released and introduced synchronous sheet metal modeling.  But again there seemed to be two separate paradigms with limited connection between the two. This all changed with the release of ST3 which introduced integrated modeling, allowing users to combine both paradigms within the same part. Unfortunately, many users had already made up their minds based on their less than successful attempts with ST and ST2.

    Another reason for resistance is lack of training. Too many companies fail to see the benefit in properly training their users in the synchronous paradigm. They expect the user to pick it up on their own, while maintaining the same level of output.  It has been my experience that this approach fails most of the time. Designers may attempt to learn it, but will often revert back to the way they know, in order to meet company deadlines. The user will often resist the change for no other reason than lack of time to properly learn it.


    The third reason is that there are some definite limitations in synchronous modeling. Certain features or techniques behave better in ordered because of the nature of synchronous modeling. I list the main Cons of synchronous modeling as follows:

    Certain features have limited editing capabilities and are handled better in the ordered paradigm. Some examples include:
    o Swept and lofted features 
    o Certain rounds and blends
    o Surfacing
    Dangling bends are not currently supported in synchronous sheet metal. This limits

    certain functionality.
    Training – users need proper training to understand the synchronous paradigm. 


    Some users may believe that they have more control in ordered, but that is a myth, based on lack of knowledge of the synchronous modeling tools. I will explain this more in my next blog article. But let me finish this article by discussing the integrated modeling approach.


    Pros and Cons of the integrated modeling approach


    Solid Edge allows the user to start the design in the synchronous paradigm and add ordered features if necessary. This approach allows the user to utilize the best of both paradigms. The synchronous portion of the model becomes the parent of the ordered features. This allows the user to change the synchronous parent which triggers an automatic update of the ordered dependent features. Furthermore the assembly can be populated with ordered parts, synchronous parts, and integrated parts. 


    The only Con for this approach is that the designer has to be trained properly.

    In my next blog article I will continue this article and further discuss the reasons why  customers are resistant to changing to synchronous technology. I will show how these perceived reasons are based on myth or inaccurate information. It is my hope that after reading both these articles you will have a better understanding of synchronous technology and be willing to take a second look at how it can be integrated into your design process, saving you time and money. 



    How to create an adjustable coil spring

    John Pearson - Wednesday, September 18, 2013
    How to create an adjustable coil spring

    If you wish to create an adjustable part, you must build a part that is adjustable. Sounds obvious, but sometimes what seems adjustable to the eye is not adjustable in the CAD system. For example, let’s look at this coiled spring.


    New users may look at the part and model it using the helical protrusion command to make the coil. Then use protrusion and/or swept protrusion to complete the part. This will look good but will not be adjustable. Why? Let’s look at the part in an adjusted or deformed state.


    Notice that the coil deforms as the part adjusts. If you model this with a helical protrusion, the rules of the helix will prevent you from deforming the coil. So how do you model this to get the adjustable results?

    There may be other ways to model this part, but I find this method fairly easy to create while giving me the control I need. I start by creating a flat sketch of my part, on the Top reference plane.



    Notice the 2 lines labeled A. These lines represent my wrapped coil center lines. My wire will be 7.5 mm in diameter, so I’ve made the opposite ends 8 mm wider, to avoid any body intersection. The 157.1 mm length of these lines is equal to the perimeter of the initial coil size. I‘ve used two tangential arcs to create the lines, because it generates a nice smooth flowing coil.

    I then create a second sketch on the Right reference plane to represent the initial coil position.


    The top quadrant is connected to the (0,0,0) point with the center of the circle horizontally aligned beneath it.

    I then create an extruded surface, which I will use to wrap the coil around. The Extruded Surface command is found on the Surfacing Tab, in the Sufaces group.



    Next, I use the Wrap Sketch command to wrap the arcs around the extruded surface. This command is found under the Surfacing tab, in the Curves group.



    I am first prompted to select the face that you will wrap around. I select and accept the extruded surface.





    I am then prompted to select the sketch that I wish to wrap. I set the selection filter to single and pick the four arcs from the sketch.



    Once I accept the selection, the arcs wrap around the extruded surface.




    To make it easier to visualize the next steps, I hide the extruded surface. I then create a sketch, to represent the diameter of my wire, centered on the top of the flat wire, on the Front reference plane.



    I then use the Swept protrusion command to create 3 features. Note: I use the following options when creating all 3 features.




    The first swept feature looks like this:



    The second swept feature looks like this:


    The third swept feature looks like this:





    Finally, I hide all sketches and curves, and then I create the last two wire sections. I could use several different methods to create these sections, but for simplicity I used the Thicken command, and simply thicken the end faces the distance that I need.


    I now have the modeled part which I can make adjustable.

    In this model we want to adjust the tilt angle of the legs, which is actually controlled by adjusting the diameter of the coil.

    To simplify the process I open the Variable Table and rename the variable that controls the diameter of the coil, to Coil_diam.



    I then create an associative sketch, on the Right reference plane, to allow me an easy way to monitor the tilt angle of the legs.



    Note: I used the Include command to create this associative line.
    In the Variable table, I located  the 90 degree variable and renamed it to Tilt_angle.



    If I change the Coil_Diam  value, I will notice that the Tilt_angle  value changes because of the associativity between the Sketch and the model.

    For example, if I change the Coil_Diam to 55 mm the Tilt_angle changes to 57.27 degrees.




    Now that I have this relationship, I can use the Goal Seek command to get the exact Tilt_angle  value, that I need. 

    I select the Goal Seek command from the Evaluate group, under the Inspect tab.



    On the command bar I input the following information;


    Goal: Tilt_angle
    Target: My desired Tilt_angle (e.g. 45 degrees)
    Variable: Coil_diam





    When I accept this input, the Goal Seek will run through a series of iterations, until it finds the exact Coil_Diam value, to give me the desired Tilt_angle value. 

    In the example, the results are as follows:



    I now have a part that can easily be adjusted, without having to create any complicated formulas.

    Note:  Clearly the deformation of the coil has it limits. If you enter in too large of a Tilt_angle, the model may fail. I have also kept this example simple; therefore if you try too many different angles, without resetting back to the original angle, the model may fail.

    It is important to note that this example could be created in several different ways and still provide you with similar results. The main thing here is that the model must have the flexibility to adjust. If I had used the Helix command instead of the Wrap Sketch command, I would not be able to adjust the coil. I can also obtain the desired results using the Goal Seek command. This saves me from having to derive complicated mathematical formulas. 




    How to copy styles from an existing document to an active document

    John Pearson - Thursday, August 29, 2013
    I recently had a technical support call, in which a customer wanted to add her own styles to the company template. She did not have access to the company templates, to change the styles, but needed to add specific styles for her current project. She wanted to know if there was a way to achieve this task without having to recreate the styles in every new document.  Fortunately the answer is yes. There is an often overlooked tool in the styles dialog called the Style Organizer. The Style Organizer tool is found on the Style dialog box.





    The following steps are used to copy a style from an existing document to your active document:

    Step 1. From the active document choose View > Style > Styles. 


    Note: This example uses images from the part environment. The steps are the same in the draft environment, but the ribbon bar looks different.

    Step 2. On the Style dialog box, set the Style Type box to the type of style you want to copy.

    For example, you may want to copy an existing Face Style that you previously created in an older document.  In this case you would highlight the Faces Styles, as shown below.


    Step 3. On the Style dialog box, click the Organizer button.



    Step 4. Browse to locate the existing file that has the styles that you want to copy.



    Note: In this example, I browsed for an existing file called Head Board.prt. Notice that all the Face Styles for Head Board.par are listed in the left side window and all the Face Styles of my active part are listed in the right side window





    Step 5. Locate and select the Face Style that you want to copy and click Copy.

    In this example I want to copy a “Wood, Cherry” face style, from the Head Board.par. I scroll down to locate the Face Style, highlight it, and then click Copy.



    Notice that the “Wood, Cherry” face style now exists in my active part file.





    Step 6. Close out of the command and use the style as you see fit.
     
    Remember, you can copy any style, such as Dimension Styles, Drawing View Styles, Hatch styles, etc. into your active document. You may have noticed that you can also delete unwanted styles, using the command.

    This is also a great tool for updating templates. If a user has created a style that he/she uses all the time, the CAD administrator can use this command to copy it into the company template. This is much easier than trying to recreate the style and also ensures accurate results. I hope you find this tool as useful as I do.

    How to show/paint individual parts/components in a draft file

    John Pearson - Thursday, July 11, 2013

    In the following example I wish to show only the weld bead as a solid in the draft view.




    To do this, I first create a Fill Style by doing the following:



    On the Home tab > Dimension group select the Styles command.



    Select Fill from the Style types: list, in the Style dialog.





    Click on the New button in the Style dialog.



    In the Name: field type in a new name, for the style. In this example I used Weld.





    Move to the Properties tab and select a desired fill color from the Solid color: pull-down list.





    In this example I selected Dk Gray. Click OK.




    Click Apply to accept the new Fill Style.




    Now I can paint the sections in the draft view by doing the following:

    From the Sketching tab > Draw group, select the Fill command.





    Select the Weld fill type, from the list in the command bar.




    Now select the enclosed areas that you wish to paint on the draft views.





    I now have a solid looking weld bead, while maintaining the wireframe look to the rest of the parts in the drawing view.






    Synchronous Assembly Modeling Boolean Commands in ST6

    John Pearson - Wednesday, July 03, 2013

    The user can now use faces and bodies from other assembly occurrences directly when executing Boolean operations for the “Tool” step such as Union, Subtract, Intersect, and Split.



    This enhancement is intended to remove the Inter-Part Copy step during a synchronous in-place activated modeling operation. Not having to create Inter-Part copies accelerates the design process and avoids the necessity of having to save the Inter-Part copies in the PathFinder.

     

    Let’s have a look at the following example:



    In this example, I have raised the motor up to show that we need to place some cutouts and holes in the underlying plate.



    First, I will edit into the Base Plate part from within the assembly. Make sure that the Hide Previous Level command is turned off in the Part environment. 



    Next, I select the Boolean Subtract command from the Solids group in the Home tab.


    You are prompted to select the target bodies for the Boolean. In this example, I select the base plate part. 



    You are then prompted to identify the tool bodies. In this example, I select the motor and the four mounting bolts, and accept the selection. 



    If we hide the tool bodies, you can see the result of the Boolean operation.



    Remember, this is a synchronous part, so we can easily add a dimension to the inner cutout and increase the size for clearance.


    We can also use the Recognize Hole command and easily convert the holes to threaded holes.


    This is just one of the many new features in Solid Edge ST6 geared to accelerate your design process, allowing for faster time to market. 


    Solid Edge ST6 Offers Multiple Version Installation

    John Pearson - Thursday, June 27, 2013

     

    Solid Edge ST6 Offers Multiple Version Installation

     

    Solid Edge ST6 now provides the user with the ability to run multiple release versions at the same time. This will allow easier testing of new releases prior to putting them into production. The earliest supported version of Solid Edge for multiple install with ST6 is Solid Edge ST4.

     


    Solid Edge Multiple Install will not allow certain combinations of the software to be installed together. For example, users will not be able to have multiple versions of MP’s (maintenance packs) installed from the same release version.

     



    Users should also not install different 32/64 Bit versions of Solid Edge on the same system.

     

     

     

     

     


    Since this new feature is designed for testing purposes, secondary applications are not fully supported with multiple installs. For example, Solid Edge Embedded Client, Standard Parts, Automated Executions, are not supported.

     

    In order to successfully install multiple versions of Solid Edge, the user must run a silent install on the latest version. Before running the silent install, a few steps must be followed:

     

    1.    When installing multiple versions of Solid Edge, it is recommended that users install the oldest version first, followed by the latest.

    2.    Ensure that you install the associated MP for the oldest version prior to installing the second version on your system.

     

    3.    Ensure that the user attempting the silent install has administrator privileges.

     

     

    Solid Edge Silent Install

     

    You can silently install Solid Edge ST6 using the following command. Be sure to enclose path names in quotes if they contain spaces.

     

    Note: Do not silently install Solid Edge if you use Standard Parts or Web Parts. These components require the .NET framework, and the .NET framework is installed only when you run setup.exe.

     

    C:\>msiexec /i “D:\CM_SETUP\DISK1\Solid Edge ST6.msi”

    MYTEMPLATE=2

    USERFILESPECXML=”K:\temp\My Docs\Options.xml”

    USERFILESPEC=”K:\temp\My Docs\selicense.dat”

    INSTALLDIR=”C:\Program Files\Silent Solid Edge\” /qn+

    /l*v “K:\temp\mysilentsetup.log”

     

    ·         The string D:\CM_SETUP\DISK1\Solid Edge ST6.msi represents the fully qualified path to the Solid Edge MSI file. The drive letter D is only an example of the drive letter for the DVD ROM. Your drive letter may be different.

     

    ·         The MSI property MYTEMPLATE indicates which type template files are to be installed. Ignoring this property defaults the installation to ISO template files.

     

    Integer

    Value

    1

    Metric

    2

    JIS

    3

    ISO

    4

    ANSI

    5

    DIN

    6

    UNI

    7

    ESKD

    8

    GB

     

    ·         The MSI Property INSTALLDIR is used to specify the installation folder for the application.

     

    ·         The MSI Property USERFILESPECXML provides the optional installation of a SE Admin file. You should supply a fully qualified path and filename. This file is copied to the Solid Edge Program folder and processed at the end of the setup.

     

    ·         The MSI Property USERFILESPEC optionally provides a license file that setup copies to the Solid Edge Program folder at the end of the setup.

     

    ·         The argument "/qn+" instructs the Windows installer to provide NO user interface and alert you at the completion of the setup using a dialog box. Refer to the Windows help system for further information about Windows Installer arguments. Leaving this argument off the command line will display the setup user interface with selections made and fields provided.

     

    Note:  If you are using this option, some installations that require user interaction could fail.

     

    ·         The argument "/l*v" tells the Windows installer to create a log file of important messages, warnings and errors and write it to the location provided, in this example, K:\temp\mysilentsetup.log. Additional information regarding logging options can be found in the Solid Edge readme.txt file.

     

    Note:  Solid Edge requires Microsoft SQL Server 2008 Express. Solid Edge setup.exe automatically installs SQL Server 2008 Express, if it does not exist on the machine. The msiexec utility, commonly used for silent install, will not install the SQL Server 2008 Express software. This must be done manually.

     

    Note: After you complete the commands on the command prompt and press “Enter” there will be no indication that the install is running. The install will run in the background until complete, in which case it will inform you whether it was successful or not.



    Set Active Solid Edge Version

     

    When running multiple versions of Solid Edge on a single machine, users will have to decide which version they will want to be active.

     

     

    Users will be provided with a SESetActiveVersion.exe tool in order to switch between active versions of Solid Edge.



     

    This will be located within the “DVD\Solid Edge\SptTools\SESetActiveVersion” directory on the installation disk. The User Interface provided with the tool will show which major release versions of Solid Edge are present on the system. To activate a different version, select the desired option from the drop down list and click “Activate”.



    Uninstalling Multiple Versions

     

    Upon completion of your testing of Solid Edge ST6, it is recommended that you uninstall all versions and reinstall the production version from scratch. The possibility of corruption of the remaining versions exists following the uninstalling of only one version of Solid Edge.




    Synchronous Hole Recognition

    John Pearson - Thursday, June 20, 2013

    If you are using the synchronous modeling in Solid Edge ST5 you may have noticed the new Recognize Hole command found under the Hole Command flyout.




    This command, specifically designed for imported models with no history, enables cylindrical cutouts to be automatically identified and re-defined as synchronous procedural hole features. It is available in the Part, Sheet Metal and Assembly environment. The user simply has to select the command and select the model. Holes are automatically recognized and displayed in the Hole Recognition dialog.


     




    Hole types and sizes are grouped together automatically.


     


    A user can choose not to recognize a cylindrical feature as a hole by toggling off the check mark for the feature.



    Within the dialog, you can rename the hole features, by double clicking on the default feature name. You can also redefine the hole feature, by applying saved settings or by using the hole options dialog.




    Once the user selects OK, to accept the hole options change, a preview of the new hole parameters is shown on the model. The user then selects OK, in the Hole Recognition dialog, to accept the change.



    The user can use the Face Selection option to recognize holes only on selected faces.




    Pre-selection of a face, or faces, is also supported. You can select a face, or faces, and then run the Recognize Holes command, to perform recognition on only the selected face(s).



    The Hole Recognition command allows users to add intelligent synchronous procedural hole features to imported models. Because it’s a hole feature, it also recognizes the user defined pattern created in all hole features, which can be used for rapid placement of bolts or screws in the assembly.