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How to Export Quality Images in Drafting

Stephen Rose - Tuesday, January 03, 2017

Introduction:

 

  • This FAQ explains the steps to generate quality shaded image views in drafting, including the use of translucency. 

 

Requirements:

 

  • Understanding of Modeling and Drafting environments in NX

 

Step By Step Process…

  •  
  • 1.Generate your solid body, or load an existing solid part, and adjust translucency as required.
  • 2.Switch to the Drafting environment and generate a sheet.
  • 3.On the top ribbon select the <File> Tab, then choose Preferences -> Drafting

 


 

  • 4.Under the <View > expandable menu select <Workflow>, then scroll down until you see the Visual Settings group in the right-hand pane.In that group check <þ> Use translucency and <þ> Use Line Antialiasing then select <OK>.(n.b. See end of document for anti-alias impacts)
  •  
  • 5.Place a view of your choice on the sheet drawing (the default will be a wire-frame view.

 


 

  • 6.Select the drafting view boundary, right-click and choose Settings
  • .
  • 7.For best results, in the left-hand pane, under the <Common> expandable menu select <Configuration> , and in the Settings group in the right-hand pane set preference to Exact Representation, rather than Lightweight.You can specify the curve tolerance here also.

 


 

  • 8.Now scroll down further in the left-hand pane and select <Shading>, and in the Format Group in the right-hand pane change the Rendering style from Wireframe, to Fully Shaded.Make any other adjustments needed for surface Shininess, then in the Tolerance group select one of the default Tolerances, or chose Customize to edit manually.Then click <OK>.

 


 

  • 9.You will then see results similar to this:

 


 

  • 10.You can then set other view dependent preferences if you want hidden lines, or smooth lines, shown different than the default setting.      Default

 

      Smooth Edges lightened

 

      Hidden lines processed

 

  • 11.Once your views are set you can use File->Export->pdf, you can use File->Print to a pdf, (with Export shaded views as wireframe left Unchecked), or you can File->Plot to plot to a suitable configured printer--or even plot out to a graphics format such as TIFF.

 

n.b.Out of the Box the Graphic Plotting format resolution is set quite low.If you need a higher resolution you can go into the plotter administration and change the values.

  •  
  • 12.To set these Graphic Formats resolutions go to File->Utilities->Printer Administration, you are then prompted to Edit the printer setup or Create a new one.(See the Plotter Setup documentation for this initial setup.)Once you are in the Edit menu, you will see the <Graphics Default> tab, under that tab are the types of graphic formats for plotting to. You can edit each of their default resolutions here.

 


 

Anti-Alias Notes in Drafting Mode:

 

Anti-alias choices can make an impact on how well your shaded surface edges show up on the drawings.The two pictures directly below show the Drafting Preference setting “Use Anti-Aliasing”

 

  

Use Anti-Alias Unchecked (OFF)               Use Anti-Alias Unchecked (ON)


 

Adjusting Full-Scene Antialiasing toggle, can also sometimes improve results.

 




NX Isocline Series.Part III of III, Mechanism Lead-in and Angled Isocline

Stephen Rose - Friday, October 23, 2015

 Overview


There are common poor-practices in the moulding industry, in this series we will shed light on some.

 

They often occur due to:

 

Lack of internal company best-practices; attempting to rush though a project to meet the common compressed deliveries of today’s industry; lack of available tools in competitor software products; lack of awareness by the designer; or sometimes due to lack of training in the functions/tools available to the designer.

 

In this series we will cover several scenarios where the right feature functions, and the right training, can create a better finished product and more stable steel conditions.Stable steel conditions allow the mould to stand up to high production volume and eliminate production downtime due to pulling the mould for repair.Having more of the finished parts being passed through QC inspection, and having less downtime of the mould, both contribute into a lower life cycle cost of the project.

 

The scenarios we are going to cover in this series include:

 

  • I)The general Isocline split
  • II)The corner contoured split
  • III)Mechanism lead-in and angled Isocline (This Entry)


What is an Isocline?


For those unfamiliar with the term Isocline, here is the dictionary definition:i-so-cline, noun, a line connecting points of equal gradient or inclination.


Where to find it


The Isocline Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Derived Curve->Extract

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or your own customized Role where you have already added the Extract Curve to your ribbon. In the Advanced Role you will find it in CURVE->More Gallery->Derived Curve group->Extract Curve

 

There is always the command finder where you can search the Isocline feature and access it directly.

 

Use:Part III, Mechanism Lead-in and Angled Isocline

 

Note:If unfamiliar with the Isocline feature and its use, please refer to Part I and Part II of this series where it is described in more detail.


Here we have a part with a full radius around the periphery of a dog-house type feature that will need a mechanism to de-mould it.

 


 

Poor-practice When Generating a Lead-in Parting-line for a Mechanism Split

 

A poor-practice when a designer creates the split line of a part is that they will generate it only in the main die-draw +Z axis.While this is the required split to have an open draft condition for the core and cavity halves, this doesn’t necessarily create good conditions for a side action mechanism.Below is an iso-view of the part with a +Z axis Isocline curve.

 


 

When using this Isocline for generating side-action mechanisms a 90° steel condition only exists if we were to extrude the curve with no draft angle.This does not work well for side action mechanisms due to the mechanism needing to have lead-in draft (also referred to as break-away angle).

 


 

The need for lead-in means the Extrusion must be drafted based on the Mechanism Pull Axis.In the picture below the draft angle has been set to 20° to illustrate a point.(Typically in the industry 5-7° is considered a good angle).

 


 

You can see with the Iso-view and the following section what this does to the steel condition on the cavity.

 

 


 

Best-practice for Generating a Lead-in Parting-line for a Mechanism Split

 

We first need to generate an angled isocline curve that will be perpendicular to the lead-in angle.This ensures that the steel condition will be 90° all around the feature.

 

Start the Isocline command.

 

1.Set the type of Vector method.

 

2.Select the axis for the Vector (In this case the - X-Axis)

 

3.Reverse the axis if necessary.(In this case we reverse it to point –X)Then click OK.

 


 

4.Set the draft angle to be the compliment of the angle we want for lead-in.In this case we want a 20° lead-in later, so we set the Isocline angle to 70° (90°-20°).Then click OK.

 


 

5. 6. 7.Select the surfaces to generate the Isoclines on.(There are options in the dialog box for selecting all faces, but in this case we are being very specific about where this parting takes place)

 

8.Click OK to view Isoclines.

 


 

This picture below shows the original +Z axis Isocline split of the whole part (Red thick line) compared to the Isoclines we now generated based on the Mechanism Pull Axis (Blue lines).Two 70° conditions exist because of the convexity of the surface.We are only going to use the outer most line for our Extrusion.

 


 

9.Select the outer Isocline

 

10. Specify the Mechanism Pull Axis (This needs to be the same as the Axis used to generate the angled Isocline.

 

11.Set the Extrusion length

 

12.Change the DRAFT option from ‘None’ to either ‘From Section’ or ‘From Start Limit’

 

13.Enter the desired lead-in angle (this is per-side, not an included angle measure).Then click OK.

 


 

You can see with the new Iso-view below and the following new section that using this method ensures the lead-in split we want splits the geometry at the true 90° position.

 

 

 

 

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly atinfo@designfusion.com.

 


NX Isocline Series.Part II of III, the General Isocline Split

Stephen Rose - Friday, October 02, 2015
Overview

 

There are common poor-practices in the moulding industry, in this series we will shed light on some.

 

They often occur due to:

 

Lack of internal company best-practices; attempting to rush though a project to meet the common compressed deliveries of today’s industry; lack of available tools in competitor software products; lack of awareness by the designer; or sometimes due to lack of training in the functions/tools available to the designer.

 

In this series we will cover several scenarios where the right feature functions, and the right training, can create a better finished product and more stable steel conditions.Stable steel conditions allow the mould to stand up to high production volume and eliminate production downtime due to pulling the mould for repair.Having more of the finished parts being passed through QC inspection, and having less downtime of the mould, both contribute into

a lower life cycle cost of the project.

 

The scenarios we are going to cover in this series include:


  • I)The general Isocline split
  • II)The corner contoured split (This entry)
  • III)Mechanism lead in and angled Isocline.


What is an Isocline?


For those unfamiliar with the term Isocline, here is the dictionary definition:i-so-cline, noun, a line connecting points of equal gradient or inclination.


Where to find it


The Isocline Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Derived Curve->Extract

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or your own customized Role where you have already added the Extract Curve to your ribbon. In the Advanced Role you will find it in CURVE->More Gallery->Derived Curve group->Extract Curve

 

There is always the command finder where you can search the Isocline feature and access it directly.

 

Use:Part II, The Corner Contoured Split

 

Note:If unfamiliar with the Isocline feature and its use, please refer to Part I of this series where it is described in more detail.

 

Here we have a moulded part with a full radius around the periphery of the wall-stock edge.

 


 

This is a close-up view of the radius following the outer wall-stock edge with an Isocline generated for the parting-split.

 


 

Common Poor Practice of Contour Split Parting-line

The common poor-practice around contoured corners typically manifests as a designer pulling off the parting-line split in the X and Y axis without regard for the shape when looking down from the plan view (die-draw axis).This often leads to poor steel conditions when the plan view has curvature and the profile has depth changes.These steel conditions can become very sharp (knife edge/feather edge) when the parting-line split is done off a ball radius.

 

Below is a Plan view (die-draw view) of poor-practice parting-split that is seen all too often.

 


 

Below is an Iso-View of the poor parting-line split.

 

Items to note are:the transition point at ‘x’ –which never gets fit cleanly and leaves a little mark on the part at that junction point; and the run-off of the parting-line split in the Y-Axis that is pulled off without regard to the shape of the part—this creates a wedge shape for the cavity steel coming in.This is better illustrated in the Section A-A which accompanies the Iso-View.

 


 


 

Below is another section cut Normal to Z-Axis just to illustrate the knife edge for another perspective.

 


 

This type of parting-line split with such a sharp steel condition has a significantly shorter life span than a well generated run-off.This type of steel condition can be difficult to fit during the manufacturing process when spotting the core and cavity halves together.During production this condition tends to get bent over and wears quickly--requiring frequent weld and re-cut / re-spot work.This raises life cycle cost of the mould, and also overtime the match edge of core to cavity tends to drift, causing more rework on the opposing half to keep the match line clean.

 

Best-practice for Generating a Robust Corner Contour Parting-split.

 

First generate the Isocline as previously described.We want to create is a parting-line split surface that extends perpendicular to the shape of the trim-edge while maintaining a flat to Z orientation.Creating this type of mould run-off ensures that any sections cut perpendicular to the contour will always be creating a solid steel condition for both the core and cavity based of the Isocline curve.

This type of run-off can’t be built by simple Extrudes since the Extrude needs a fixed axis.The designer could do some Extrudes for areas that are aligned with the X or Y axis and then manually build smooth surfaces to transition around the corner-- connect tangentially to the two Extrudes. Manual operations can be time consuming, so in this case the two best options we have are Law-Extension surface, or Ribbon Builder.Both features can be set to create an almost identical desired output.

 

Law Extension Method

 

The Law-Extension Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Flange Surface->Law Extension

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or if you are in the Essentials Role you will need to first add the Surface Ribbon tab to the top interface by right-clicking and setting the check-mark for Surface.Once your Roles and Ribbon are set you will find it in SURFACE->Law Extension

 



 

 

With the Law Extension dialog box open:

1.Set the Type to Vector method in the drop down option.

2.Select your previously created Isocline curve(s)

3.Set the vector option to be the +Z die-draw axis.

4.With the Length Law-type set to constant, enter a value for how long you want the surface extension to be.

5.With the Angle Law-type set to constant, enter 90° (or -90° if curve direction forces surface to extend the wrong direction.)

Then click OK and a surface is build °90 from the die-draw axis which follows the contour of the part.

 


 

 

Ribbon Builder Method

The Ribbon Builder Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Surface ->Ribbon Builder

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or if you are in the Essentials Role you will need to first add the Surface Ribbon tab to the top interface by right-clicking the border for the tabs and setting the check-mark for Surface.Once your Roles and Ribbon are set you will find it in SURFACE->Surface Group->More Gallery->Ribbon Builder.

 



 

With the Ribbon Builder dialog box open:

1.Select your previously created Isocline curve(s).

2.Set the vector option to be the +Z die-draw axis in the drop down list.

3.Set the ribbon extension length as needed.

4.Set the angle to 0°

Then click the preview option to see if that ribbon is created as desired, click OK if it is, and a surface is built that is 0° Normal to the +Z axis of die-draw.

 


 

Using either method shown above to generate a run-off surface from the Isocline results in a split-surface that separates the core and cavity halves at the split of the radius. It also follows the curve path so that the extension/ribbon is created close to perpendicular to the plan view orientation.This ensures the steel condition is consistent and does not exaggerate sharp corners by the designer arbitrarily determining which vector direction to pull the surfaces off of -- as seen in the poor-practice example near the top of this article.

 

Below is our result, and the pictures following show the superior steel condition created as a result.

 


 

Below is an Iso-View and Section view cut perpendicular to the Isocline curve.

 



 

Below is an Iso-View and Section View of a section cut through the vertical wall transition

 



 

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly atinfo@designfusion.com.

 


NX Isocline Series.Part I of III, the General Isocline Split

Stephen Rose - Wednesday, September 23, 2015

Overview

 

There are common poor-practices in the moulding industry, in this series we will shed light on some.

 

They often occur due to:

 

Lack of internal company best practices; attempting to rush though a project to meet the common compressed deliveries of today’s industry; lack of available tools in competitor software products; lack of awareness by the designer; or sometimes due to lack of training in the functions/tools available to the designer.

 

In this series we will cover several scenarios where the right feature functions, and the right training, can create a better finished product and more stable steel conditions.Stable steel conditions allow the mould to stand up to high production volume and eliminate production downtime due to pulling the mould for repair.Having more of the finished parts being passed through QC inspection, and having less downtime of the mould, both contribute into a lower life cycle cost of the project.

 

The scenarios we are going to cover in this series include:


  • I)The general Isocline split (This entry)
  • II)The corner contoured split
  • III)Mechanism lead in and angled Isocline.


What is an Isocline?


For those unfamiliar with the term Isocline, here is the dictionary definition: i-soc-line, noun, a line connecting points of equal gradient or inclination.


Where to find it

 

The Isocline Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Derived Curve->Extract

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or your own customized Role where you have already added the Extract Curve to your ribbon. In the Advanced Role you will find it in CURVE->More Gallery->Derived Curve group->Extract Curve

There is always the command finder where you can search the Isocline feature and access it directly.

 

Use: Part I, The General Isocline Split

Here we have a moulded part with a full radius around the periphery of the wall-stock edge.

 


 

This is a close-up view of the radius following the outer wall-stock edge.

 


 

Common Poor-practice for Building Parting-line Split

The common poor-practice seen in the moulding industry is pulling off the parting-line split from the edge of the radius.Typically this is seen on somewhat vertical walls where the low draft angle doesn’t show much deviation from the radius edge to the true tangent apex of the radius (as compared to the die-draw).

 


 

From this close-up section below (and using iso-view above) you can see the designer selected the radius edge as the split for the mould.However based on the vertical die-draw axis (+Z) you can see that the radius actually bulges out past this split point to become slightly under-cut to die-draw.This causes a die-lock condition for the moulded part.

 

Several reasons why this goes unnoticed in the manufacturing process can be attributed to, but not limited to:

 

A)The undercut condition is very small and as the moulded part shrinks it releases itself from the under-cut and is no longer die-locked.

 

B)The mould was cut vertically in the Z axis so the cutter never actually cuts in the under-cut condition—thus leaving the customer with a blunted radius.

 

C)The mould is cut as shown but during hand polishing operations the top lip of the core is polished away leaving open draft—This then creates a mis-match condition where the core steel is stepped out past the cavity edge, and then polishing of the cavity edge is necessary to bring it over to the new core position.

 


 

Best-Practice for Building Parting-Line Split

First enter the Extract menu from either the traditional Menu button or through the Ribbon interface and choose Isocline.

 

Menu button:

 


 

Ribbon Interface:

 


 

Once in the Isocline dialog box:

 

1. We select the die-draw axis either using the default inferred vector selection, or any of the options in the Vector drop down list.If necessary you can then use the reverse vector orientation option. Note:after selecting the axis the dialog still shows 0 for the selection even though you have defined it, at this point hit OK to accept the vector selection.

 


 

2.In this case we make sure the Single option is selected as we only want one set of curves.(The family option lets you generate multiple sets of curves between a range and angle step over.)

 

3.We then set the angle requirement--from the die-draw axis-- to create the isocline at.In this case when creating the outer parting split normal to the +Z axis we set this value at 0°.Then click OK to accept the angle and progress to the face selection dialog.

 


 

4.We then select all the faces we wish to process for Isocline creation.This can be done by single on screen selections, or the other selection options presented in the dialog box.Depending on how you intend to use the Isocline command in your process you may want to select all faces in body if you think the data will change enough that all faces need to be processed, however if you are quite sure it will only be these local faces to be accommodated then it’s best to only select the needed faces to reduce the amount of faces processed during updates.After selecting the faces needed in this set click OK.

 



You will be returned to the first Isocline menu again in order to create further Isocline definitions, but in this case click Cancel.

 

An Isocline representing the parting-split is generated (Red Line below).You can see the difference between A) the original radius edge, and B) the position of the Isocline split.

 


 

We now can develop a parting-split surface from the Isocline curve.

 


 

From this close-up section below (and using iso-view above) you can see that the parting-split surface lies at the 0° draft location of the radius and that the split now represents the outermost extent of the radius surface data.This split location ensures open draft to each half of the Core and Cavity.

 


 

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly at info@designfusion.com.





NX Draft Feature

Stephen Rose - Wednesday, July 29, 2015

Overview


Most users are familiar with the need to draft walls of parts or tooling to a certain angle. For those that are not familiar: It is used in manufacturing to allow de-mold of plastic parts and castings, a design requirement of some sort of functional fit, or so that the cutter and possibly the holder have clearance when machining down in deep-draw cavities.

 

The NX Draft Feature command has different sub-types when applying draft angle to a model.In this example we will use the two simplest types From Edges and Tangent to Faces types.

 

Where to find it

 

The Draft Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Detail Featureà->Draft

 

If you are more comfortable with the NX Ribbon style interface you will find it in HOME->Feature Group->Draft

 

There is always the command finder where you can search the Draft feature and access it directly.


Use


Here we have an unfinished (yellow) part with vertical side walls as our starting body.First we want to add a simple draft angle to the side walls.

 


 

We access the Draft Feature command, either from the Menu or the Ribbon Bar interface.

 


 

Ribbon Interface

 


 

Once in the Draft Feature:

 

1. We select Type of Draft from the drop-down list and pick From Edges.

 

2.We define the Draw Direction, in this case the Z axis.

 

3.We proceed to select the bottom periphery edge of the part.

 

4.We set the angle to 5° and then with the preview option turned on we see the model updates to having 5° draft around the entire edge.(NX is smart enough adjust the upper radii

without the need to remove the radii and reapply after the draft command.)We use OK to apply this draft and exit the dialog box.

 


 

With the body drafted we now want to add a Hole Feature.In this example we set the Counter Bore Diameter large enough, and the position of the hole far enough over, so that the Counter Bore breaks out the side of our body.

 


 

With the C’bore subtracted the resultant part shows that there would be sharp material conditions where the holes break out the side of the body walls.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)

 


 

We want to clean up this condition by straightening the C’bore surface so they end up breaking out 90° to the side walls.

 


 

We enter the Draft Feature once again:

 

1. We select Type of Draft from the drop-down list and pick Tangent to Faces.

 

2.We define the Draw Direction, in this case the axis must point away from the concavity of the c’bore-Y axis (not into it as +Y) as indicated by the orange arrow .

 


 

3. We then select the C’bore face that is to be drafted.

 


 

4.We set the angle to 0° and then with the preview option turned on we see the model update to having 0° draft to the axis, but starting tangent to the C’bore face.

 


 


 

After hitting OK to accept the draft we end up with the modified part body as shown.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)

 


 


 

This type of modification can be very useful in part/product design to clean up features and eliminate sharp corners in a mold. It can also can play a part in the tooling industry by opening up areas for milling machines. Opening up various break out areas on tooling can increase the amount of machining strategies available to complete a particular feature.In this case access to the side of the feature is now possible.Efficiency could be realized by allowing use of profile or other machining methods to complete the majority of this part, rather than having to mill down the vertical axis of the feature only.

 


 


If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly at info@designfusion.com.



How-to create a reference in draft from the assembly

Charles-Etienne Lavoie - Tuesday, August 12, 2014

How-to create a reference view in draft and keeping associativity to your assembly.

 

1) Place the assembly has you would normally do in a MASTER MODEL draft,

 

 

 

2) To create the individual views, return to the MODELING environment.

 

 

 

3) Open the exploded view menu




4) Orient the view to the desire position and save as

 

 

 

 

5) From the exploded view menu, select hide component to hide the unwanted part




6) Hide the component

 

 

 

7) You can use the show component in view to show component

 

 

 

 


8) Save the work view when done

 

 

 

9) To change the work view to a canned view, RMB in the work environment and select replace view, from there select any view or use custom for a more specific view.

 

 

 

10) Return back to the drafting environment and add the newly create view to your sheet

 

 

 

 

 

 

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. 




NX – Create a family of standard parts (Excel)

Charles-Etienne Lavoie - Wednesday, July 04, 2012

                   

                  Design Intent:


                  The most common use of Part Families is to define a standard library part that has many variations.


                  1. Create a hexbolt 

                   


                   

                  2. Rename the expression that you want to keep


                  •   a-Width = the radius of the cap

                    b-Length = length of screw

                  •  

                  3. Define the columns for the Family Table.

                   

                    Choose Tools→Part Families from the main menu bar.

                    Make sure the Importable Part Family Template option is cleared.

                    Click OK on the Warning dialog box.

                    Select the width expression from the top window of the Part Families dialog box.

                    Click the Add Column button.

                   



                    Select the length expression from the top window of the Part Families dialog box.

                    Click the Add Column button.


                  Note:

                  Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.

                   

                    Change the option menu at the top of the dialog box from Expressions to Features.

                    Double-click chamfer from the top list of the Part Families dialog box.


                  Note:

                  The order in which you select the attributes determines the order of columns in the spreadsheet.


                  Tip:

                  In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.


                  4.Create the family table.

                   

                  •   Click the Create button from the bottom portion of the Part Families dialog box.

                   


                   

                  •   Type in a few values



                  5.Verify a family member

                   

                    Select a cell in row 3.

                    From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.

                   


                   

                  The NX session becomes active and the family member is displayed in the graphics window.

                    Click Resume in the Part Families dialog box.


                  Warning:

                  The Part Families dialog box may be obscured, if so, click anywhere in the NX window.


                  6.Save the Part Family and the template part.

                    From the spreadsheet menu bar, choose PartFamily→Save Family.


                  Note:

                  The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.


                  Note:

                  In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.

                   

                  Since we do not use this part anywhere else we are not going to do that.


                  7.Close all parts.