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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.

Solid Edge ST6 introduced at SEU2013 – Part 1

John Pearson - Friday, July 12, 2013

In the last few blog articles I have highlighted a couple of enhancements coming in Solid Edge ST6. Having just returned from Solid Edge University 2013 (SEU2013), where customers were introduced to Solid Edge ST6, I thought I should try and list some of the more than 1300 enhancements. Clearly, with over 1300 enhancements, it would be a major job to list and discuss all the changes, so I will only highlight some of the major improvements.


Before looking at some of the new features in Solid Edge ST6, I think it’s worth mentioning that in Q2, Solid Edge license business in the US has seen a 25% year over year growth. Combine this with the growing number of packages that work with Solid Edge; it is clear the Siemens is fully committed to the continued growth and success of Solid Edge.


Some of the new partners introduced at SEU 2013 include CAMWorks for Solid Edge, KeyShot and CRABCAD, just to name a few. I found the CAMWorks for Solid Edge to be the most intriguing new partner. It allows for machining of your Solid Edge model directly in the Solid Edge package. I will discuss this in future blog articles once I have been fully trained on this new package.



It was also clear, to the over 500 users that attended SEU2013, that Siemens is listening to their customers. As I mentioned earlier, Solid Edge ST6 satisfies over 1300 customer requests. This is the breakdown as presented to us at SEU2013:




So what did I find to be the most intriguing new features? First, I really like the new ability to install multiple versions on the same computer (see earlier blog article on how to set this up). Although this is for test purposes only, it will go a long way to allowing smoother upgrades, especially for smaller companies. Solid Edge ST6 also adds some new user experience tools, such as:


New user persona environments - to customize the user environment based on his level of expertise with the software.


YouTube in Solid Edge - The YouTube search and upload feature within Solid Edge ST6 allows you to upload pre-recorded videos, or record your own video within the UI and upload it directly through the Solid Edge application.


Record Videos in Solid Edge - Solid Edge ST6 provides the ability to record design workflows within the application.


Command Finder Updates - Enhancements have been made to the Command Finder to provide the user with additional information for searched items that are not considered Solid Edge commands.

 

Android Tablet Viewer - Solid Edge now has an App available to view part, sheet metal, and assembly files on an android powered tablet. Similar to the iPad App introduced in ST5.

Combine these new tools with enhanced learning tools and the expanded Solid Edge community, and you will find the overall user experience is greatly improved.


ST6 Surface Modeling


Some major improvements in Part modeling also impressed me and many of the other users at SEU2013. My favorite enhancements include the following:


Major overhaul of the Surfacing environment

  • ·         New easy-to-use 3D surface control handles for on screen edits of curvature with graphical            magnitude handles and numeric values.
  • ·         Key-point curves now with C2 support.
  • ·         Robust bounded surfaces also with C2 support.
  • ·         Blue surface command now has C2 handles and optional curvature combs.
  • ·         Trim and extend is now a single super command.
  • ·         Ruled Surface command added - allows the user to pick a curve and
  •        generate a sweep of linear cross section along a curve or edge.
  • ·         Redefine Surface command added - that allows a surface or group of adjacent surfaces to            be replaced with a single editable BlueSurf.
  • ·         Model Reflective Display - a new display mode has been introduced specifically designed            for studying curvature and volumes of surface models of symmetric parts.
  • ·         Plus so much more to allow users to model highly aesthetic consumer products.

There are many more improvements to mention, and I will continue to do so in next week’s blog.



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.


Integrated Modeling in Solid Edge

John Pearson - Monday, November 19, 2012

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses

Editing Part/SM Operations in Assembly

Cory Goulden - Monday, November 05, 2012
In ST5 you can now perform edit operations, from the assembly environment, without first in-place-activating to enter the model directly.  Things you can do:

• Locate, select and edit of ordered features
• Edit synchronous procedural features
• Delete synchronous face-sets and ordered features
• Move face-sets (sync feature) in synchronous parts

Let’s take a look!

Firstly, ordered features are now selectable via the Face Priority select option. (remember hotkey combo is CTL + Spacebar)

Notice in the example below that “Protrusion 1” is available from the Quickpick options in assembly now.


Once selected, “Protrusion 1” has its options displayed for going directly into the features parameters.



Select whatever you would like to edit and SE will take you directly there.  Once complete, just close and return.  This will take you back to where you were in the assembly.

This saves time from previous versions by allowing you to go directly to what you want to modify and brings you back to the assembly reducing the number of mouse clicks.

Editing synchronous procedural features from the assembly level does not in-place-activate the user into the part.  Procedural features are things such as Patterns, Thin wall, Helix, Hem, Dimple, Louver, Drawn cutout, Bead, Gusset, and Etch.  These are editable directly in the assembly.

Using Face Select again, “Louver 1” is selected.
The handle for the procedural features shows up.  If selected we are presented with the following options.

Also, if we were to select the adjacent lover we would be presented with the following options:

Notice that the option to edit the pattern is there.  I know what the usual next question would be “How would I know how to edit the parent of the pattern?”.  Notice the option for “Louver 14”.  If you were to select it, you would be presented with the same options as previously mentioned.



We select “Pattern 1” and now we can modify the parameters that define the pattern.

Once selected, click on the PMI callout “Pattern 2 x 4” and we will get the following options:


Notice we have not left the Assembly environment.
One thing to note about this type of editing: Procedural Feature profile editing requires in-place-activating first.  Also, there is no access to the profile handle from within the assembly.
Happy Edging!

If you would like to learn more about “What’s New in ST5”, stay tuned for our new Update Training course.

Using a Quick Query in Assembly

Cory Goulden - Tuesday, October 16, 2012

Over the years I have noticed some gems in Solid Edge that I would like to share.  Quick Query I feel is a small but powerful little nugget.   I will list the steps below to perform a quick query in assembly and also try to state some benefits to this.  Trust me it takes longer to explain than to do.

Firstly it is important to note that parts and assemblies have properties embedded in them.  These fields should be used for a multitude of reasons from parts lists to searches.  It would be important for all to understand this before moving on.  Obviously these fields must have information in them in order for Solid Edge to report back anything.

Below I have an example part that exists in the example assembly I will use.

To check the properties

We can check what has been entered by going to the part properties.  Select the Solid Edge application button and go to Properties>File Properties.

You can also look at the property manager, which will be discussed at a later date, or perhaps through automation if you have a custom program to assist in entering this data.

 

As you can see below we have an entry of “hardware” in the “Category” field.  This is what we will perform a quick query on later.

We now return to the assembly.

 

Click on the “Select Tools” tab. 

Perform a quick query


RMB in the blank area just below the words in the title bar that say “Select Tools” and the following menu appears.  Note that these options correspond to those fields we had seen in the part properties.  You can set up a search to find these items based on these same categories.


 

You can see the many choices presented to you for searching.  Any one of them can be used.  For this example we will search the “Category” field.

Let’s set up a Quick Query to find and part in the assembly with the word “hardware” in the “Category” field.  We RMB in the blank area, and select “Category”.  This sets the Quick Query option to search the “Category” field in all parts and select and highlight all that contain the word “hardware”.

Once the text has been entered, press the enter key and you should have all the parts highlighted and selected like below:

Note that the highlighted parts are any that contain the word “hardware” in the “Category” field.  This search went into sub assemblies and patterns to select items.  It would also select different items as long as the field had the word hardware in it.   You could do a “Show Only” or other options for the selected set of parts.

There are many applications for this tool (another time we will discuss a full Query).  Quick Query is very useful.  It can select a set of items so you can do things like double check quantities or locations.  Also, because it shows only items matching the query, it can help determine if an item might also be missing properties.  This is good to know especially if those fields are required for a parts list in draft for example.