North America's Leading Siemens PLM Partner

Designfusion Blog

More control over the tool axis in NX11.0.1

John Pearson - Wednesday, May 24, 2017

 

Two weeks ago, I had the privilege of attending a Cam Forum for Siemens PLM Software partners. A colleague and I drove down to Troy, Michigan, where we were introduced to new NX CAM functionality in NX11.0.1. We also saw some of the future enhancements coming in NX11.0.2 and beyond. Although there were many enhancements that I could discuss, there was one in particular that I found extremely useful. So rather than give a brief overview of all the enhancements, I will focus on one of my favorite enhancements. Once you’ve loaded NX11.0.1, open the help docs and view the what’s new section, if you’d like an overview of all the enhancements.

 

 

Interpolate Tool Axis Enhancements

 

Prior to NX11.0.1, if machining the part below, with the tool shown, you’d have a tool holder collision issue along the wall.

 


 

When situations like this occur, NX now provides a new Control Direction option, when using the Interpolate Vector tool axis option. To access this new option, expand the Tool Axis section, in the operation template. With the Axis option set to Interpolate Vector, click the Edit icon.

 


 

Notice the new Control Direction option under the Interpolation Method.

 


 

The U and V option retains the behavior from previous releases. The U option controls the tool axis in the U direction only. The V option controls the tool axis in the V direction only. These two options give the new behavior.

 

In this example, I’ll select the U from the Control Direction list.

 


 

Notice the two iso curves. Each iso curve contains a system defined vector at each end. Only one vector is now necessary to define the tool axis along each iso curve.

 


 

There is another new option, that allows us to select a system defined vector and tell the system not to consider it, when interpolating the tool axis. You do this by selecting the vector, and selecting the new Ignore Point check box. In this example, I first select vector 4, from the list.

 


 

Note: You may also select the vector by single-clicking in the graphics display. Double-clicking reverses the vector direction.

 

I then select the Ignore Point check box.

 


 

I repeat this step for vector 2.

 


 

Next, I select vector 3 and use the dynamic axis handle to rotate the tool about the YC axis, until the holder no longer collides with the part.

 


 

The third enhancement becomes apparent will doing this rotation. In previous releases, the tool was rotated about the tool tip resulting in the tool cutting below the part surface. The tool now rotates about the contact point and no longer violates the part. See the image below.

 


 

When I verify the tool path, I notice that the tool holder no longer collides with the part wall, but the tool axis begins tilting sooner than necessary. This is because NX tilts the tool axis continuously as it interpolates the tool axis between the two U curves.

 


 

I can add another iso curve to control how long the tool remains vertical before tilting. To do this I return to the Tool Axis section and click Edit again. In the Interpolate Vector dialog, I select the Add New Set icon.

 


 

Next, I select a point on the edge of the part, in the approximate position shown below.

 


 

This defines an additional iso curve with a vector that can be used to control the tilt of the tool. By leaving the ZC vector vertical, the tool axis will remain vertical as it approaches the wall until it reaches this curve.

 


 

This time, when I verify the tool path, the tool axis remains vertical until it reaches the added iso curve. It then begins to tilt as it approaches the next iso curve.

 


 

As you can see from this example, you can now specify either a U or V control direction and ignore system defined vectors, allowing you to interpolate the tool axis for variable axis operations along U or V iso curves, with as little as a single interpolation vector for each curve. This capability greatly simplifies the task of specifying a constant tool axis orientation along the entire U or V curve.

 

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.

 




Moldwizard Series

Stephen Rose - Thursday, October 06, 2016

Check out our 3 part MoldWizard Series

 

Part 1:

 

 

Part 2:

 

 

Part 3:

 

 

 

NX CAM: Options for selecting cut areas

John Pearson - Thursday, May 26, 2016

 

With the daily grind to meet production schedules, it is often difficult to keep up with all the changes to NX CAM software. I have spoken with many users who are basically still using methods that they learned from their first CAM course(s), despite the fact that there now exist more efficient ways of doing things. The primary reason for this is that they have not received any update training. Some companies expect the users to learn on their own, yet fail to provide time to do so. Others don’t see the value in upgrade training, or insist that their users simply don’t need it. Whatever the excuse, training always seems to be the lowest priority, until issues arise. I have even known companies who have even investigated changing software, when the far less expensive option of training would provide them with all that they need.

 

With this in mind, I thought it may be ideal to review some of the newer and more efficient ways of doing things in NX CAM. For this blog article I’d like to focus on the new options for cut area selection, added to the fixed and variable contour operations, in NX9. You can now define Cut Areas, for these operations, by selecting a seed face and bounding edges that form a closed loop.

 

Example 1 : Let’s start by looking at a simple example where I use a seed face inside a single loop. Here I have a Contour Area operation for the part you see below.

 


 

I start by selecting the Specify Cut Area option. I then use the new selection method that has been added. This method is labeled as Edge Bounded Region, and is found in the Selection Method list.

 


 

With this new option selected, all I have to do is select a seed face, as shown below.

 


 

Then I select the bounding edge as shown below.

 


 

Tip: To ensure the selection of the tangent curve, I make sure that the selection intent, on the Top Border Bar, is set to Tangent Curves .

 


 

I then click on Preview Region, and notice that I have selected this entire region with minimal mouse clicks.

 


 

Example 2: This example shows the selection of a single seed face that is found between two containment loops. Using the same part and operation as in Example 1, I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. This time I select the seed face shown below.

 


 

As before, I use the Tangent Curves selection intent to select the top closed loop.

 


 

I then select the bottom closed loop.

 

 


 

These two closed loops form the exterior and interior containment loops and when I select Preview Region , I am shown the selected area.

 


 

If you expand the Region Options on the Cut Area dialog, you will see 2 other options, the Traverse Interior Edges option, and the Use Tangent Edge Angle option.

 


 

The next two examples will look at these options.

 

Example 3 : Using the Traverse Interior Edges option.

 

In this example, I expand on Example 1, where I have already selected the faces as shown below.

 


 

But in this example, a boss and an additional edge blend has been added to the model.

 



 

If I use the same selection method as in Example 1, but also toggle on Traverse Interior Edges, the Preview Region shows me the following selection area.

 


 

Example 4 : Using the Use Tangent Edge Angle option.

 

In this final example, I have modified the part by removing the top edge blend. By removing the edge blend, the normal vectors between the faces now form a 30-degree angle.

 


 

I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. For my seed face I select the bottom face.

 


 

For the bounding edge I select the four exterior edges shown below.

 


 

Next, I toggle on the Use Tangent Edge Angle option and set the Angle Tolerance to 25.0000, as shown.

 


 

When I generate my operation, I notice that the top planar face is ignored. This is because the normal vectors between tangent faces exceed the specified 25-degree Angle Tolerance, therefore the adjacent face is not included in the cut area.

 


 

Rule: If the normal vectors between tangent faces equal or exceed the user specified Angle Tolerance, the adjacent face is not added to the contained area to be machined.

 


 

As you can see, these new options are more efficient than the previous method for selecting a cut area. And this is just one of the many new tools added in recent years. NX CAM continues to improve its technology, but it is up to you, the user, to learn about these improvements. It has been my experience that this does not happen unless the user is allowed the time to learn. The most cost effective way for users to improve is through professional training. Update and custom courses are available through either Siemens Training or through Designfusion. For more information, contact your Account Manager or contact us at info@designfusion.com.

 

 


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 Emboss Body Feature

Stephen Rose - Tuesday, August 11, 2015

 

Overview

An often overlooked feature in NX is the Emboss Body. The Emboss Body can simplify the process when designing a part that may need to be adjusted to suit surrounding parts—a process which would otherwise require multiple steps and the use of several unite, trim, and subtract commands to accomplish the same design goal.

 

The power of the Emboss Body is not only the simple ability to impress the shape of another body into the part you are designing, but also the complex ability to specify offsets and thicknesses to rebuild the wall-stock of the part being embossed.

 

Where to find it

The Emboss Body can be found several ways. If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Combine->Emboss Body

 

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 Emboss Body to your ribbon. Then you will find it in HOME->Feature Group MORE->Combine Group->Emboss Body.

 

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


Use

Here we have a simple (yellow) molded part developed using the shell command with structural ribs and boss feature added.

 

 

Now in this example the assembly this part belongs to has another part (shown grey) that interferes. (See grey dome protruding through into back side of boss, rib and wall-stock in picture below). So we need to remodel our (yellow) part to accommodate this body. Traditional modeling techniques of modifying the (yellow) part involved building surfaces from the intruding part, offsetting for clearance, building new wall-stock then stitching surfaces or doing Boolean operations on all these to get back into one body. The Emboss Body handles all this for us.

 

 

 

Now let’s take a closer look at the interference using our Clipping Section Editor (Ctrl-H). Setting the clipping plane through the boss center we can see how the interfering part intrudes into our (yellow) part. Also note in this example we’ve set the two options for better clarity. Under the CAP settings we’ve turned on Show Cap and also turned on the Show interference and set the interference colour to Red. We’ve also turned on the Section Curve preview settings and set the section colour to Black to contrast the wall-stock. With the interference setting and section curves set it gives us a clearer indication of the interference that is happening.

 

 

 

We now enter the Emboss Body via the Menu or Ribbon Bar method.

 

 


 

We select our (yellow) part as the target, and the (grey) interfering body as the tool. With the Thicken option unchecked, and the tool clearance offset set at 0, the results we get are similar to a simple Boolean subtraction. Note: This is not how we want to develop our final part. This is just to illustrate how the options work and the differing output achieved.

 

 

 


 

In order to get our part constructed without the void that the previous views showed we need to check the Thicken option and set the value to the wall-stock that we want created. We also want to set a clearance offset zone so that the parts don’t contact each other.

 

 

 


With a couple of finishing radii and fillets the part is now complete with clearance to the intruding part and proper adjustments to the wall-stock at the ribs and boss features.

 

  

 

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 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 do you Change the Default Settings in the Operation Templates

John Pearson - Wednesday, April 22, 2015

 Manufacturing software has come a long way over the years, and it continues to improve as the machines and hardware evolve. However, the software may not be designed to handle your specific task. It is often necessary to modify settings in the operations to meet your specific needs. For example you may have to modify the cut pattern, the step over distance, cut depths, speeds and feeds, etc. If you find yourself constantly modifying settings, you may want to look at customizing your CAM software.


If your software is NX CAM Express, you can customize the package using several tools. The nice thing about these tools is that you do not have to be a code writer to use them. NX allows you to customize your CAM package in the following ways:

  •  
  • 1.Customer Defaults For Manufacturing

2.Manufacturing Templates

3.Definitions of Output formats

4.Definitions of libraries and library data

5.Process Assistants

 

Further details on these topics can be found in the NX CAM help documents, but for this blog article I’d like to focus on one of the more common requests, that I get on our tech line. How do you change the defaults settings in the operation templates? Believe it or not this is one of the easier things to do in NX CAM. However it does require some knowledge of the inner workings of NX CAM Express.


NX CAM Express Setups

 

Normally you start your manufacturing program by launching one of the pre-defined setup programs. For example, you may select the Machinery Express setup in Metric.

 

 

 

This opens the manufacturing environment, creates a manufacturing assembly and loads the Machinery Express operation templates. It knows what operation templates to load from this file:

 

C:\Program Files\Siemens\NX 9.0\MACH\resource\template_dir\template.dat


If you open this file in NotePAD, and view the list, you will see the line for the Metric Machinery Express setup.

 

 

 

The rest of the line lists the operation templates part files which NX will load for this setup.

 

 

 

The metric part files are stored in the following location:

 

C:\Program Files\Siemens\NX 9.0\MACH\resource\template_part\metric\


If you wish to change the defaults in the operations templates, these are the files you must edit.


Note: NX 9 added a new folder for updates. This folder contains the updated copies of the operation templates when you install a QRM or patch. The folder is:


C:\Program Files\Siemens\NX 9.0\MACH\updates\template_part\metric


The option to ignore this updated file is found in the Customer Defaults, under Manufacturing - General. If toggled off the original files are loaded.

 



Changing the defaults


So now that we know where the operation template files are saved, how do we edit them? Referring back to the template.dat file we see that the name of the file we need to open is the Machinery_Exp.prt. So we open the Machinery_Exp.prt found in the C:\Program Files\Siemens\NX 9.0\MACH\resource\template_part\metric\ folder.

 

Notice the Operation Navigator of this file lists all the operation templates that we can choose from when we attempt to create an operation under this setup.

 

 

 

Lets assume that we want to change the cavity mill default Stepover from a 50% to 75%, of the tool flat. To do this we open the CAVITY_MILL operation and change the Percent of Flat Diameter to 75, as shown below:

 

 

 

Click OK to close the operation. Now you must save the change. However this is most likely a “Read-Only” file, and even if it’s not, it’s a good idea to keep the original file. Therefore I recommend that you save it as a unique file. For example, I save mine as DF_Machinery_Exp.prt (DF for DesignFusion, in case you’re wondering).

 

Next I have to tell the system to load this new file when I launch the Machinery Express setup. So I open the previously mentioned Template.dat file and modify the name of the file to match my new name, as shown below.

 

 

 

I then save and close this file.

 

Testing the new settings


To test that the new default setting is working, open a new part. Run the Machinery Express setup in Metric.

 

 

 

Create a new cavity mill operation.

 

 

 

If you’ve done it correctly, you should see the new default value appear, as shown below.

 

 

 

Keep in mind that it’s always good to keep a back-up of the original files and your modified files.

 

I know that editing installed files can be intimidating to some users. For this reason, Designfusion offers customization services. If you’d like us to provide this service for your company, please contact your Account Manager, or contact us at info@designfusion.com.