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How to save a flat pattern as a .dxf file in Solid Edge

John Pearson - Monday, October 26, 2015

In this blog, I want to focus on a single command; that being the “Save As Flat” command. I receive many calls from customers who ask how to create DXF files of their flattened parts. They need them to send to their manufacturing software or machine controller. Some have become creative and make a draft of the flat pattern and save that as a DXF file, but there’s an easier and better way. The best way is to use the “Save As Flat” command, using the following steps:


Once you have your sheet metal model created, create your flat pattern.I’m assuming that you already know how to create a flat pattern, so I won’t go into detail here.

 

 


 


Technically you can use the “Save As Flat” command to flatten the part, but I always recommend using the Flat Pattern command, to do this, for 2 reasons. First, you can verify that the flat pattern is feasible, and second, you probably need it anyway for your draft document.

 

Once you’ve created a flat pattern of the model, select the “Save As Flat” command from the pull down Application menu.

 


 

Notice that the “Save As Flat” dialog appears.

 


 

Before saving the file, click on the Options button, at the bottom of the dialog. This will launch the “Save As Flat DXF Options” dialog.

 


 

This dialog allows you to control what is output to the DXF file and how it is output. For example; if your controller does not like the bend centerlines output, you can block this by unchecking them in the Export to DXF column.

 


 

Now the centerlines will not be output to the DXF file when you save it.

 

Notice that there are 3 tabs in the dialog.

 


 

You can control Layers, Bend Data, and Fonts. If you are unsure of the settings you need, check with the machine operator or machine manuals. These settings are here only for controlling what is output into the DXF file. Therefore they have to match what your machine needs in the DXF file. If you want to read more about the options dialog, you can click on the Help button, in the bottom right corner of the dialog.

 

Once you set the options, click OK to return to the “Save As Flat” dialog. Select the folder that you want to save the file in, give the file a name, and make sure the “Save as type:” option is set to AutoCAD (*.dxf), then hit Save.

 


 

You now have a DXF file, of your flat pattern, to use in your manufacturing software or send to your machine controller.


Note: Once you set the options, in the “Save As Flat” dialog, they remain set. However it’s a good idea to document the settings in case your computer fails or you move to a newer version of Solid Edge.

Feel free to experiment with the options settings. Remember these settings only effect what’s output to the DXF file. They have no effect on the Solid Edge file.

 


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.





QuadriSpace - Technical docs simplified

John Pearson - Thursday, September 17, 2015

It’s always been a tedious task to generate technical documents for any product. Often you’ll have to save numerous images or screen captures. You may even take digital pictures. Then you have to insert these into Word, Publisher, or some similar editing software, and try to blend the images and text into a usable technical document.


Over my many years in the industry, I’ve seen numerous approaches taken to generate some very specific and necessary documentation. There are packages out there that claim to do a lot of this work for you, but some require an additional seat of CAD software, for your documentation department. Others organize the process but don’t really simplify it. For the last few years, Designfusion has been looking for easy to use, affordable, interactive documentation software, to meet our customer’s needs. QuadriSpace seems to meet everything that we’ve been looking for in documentation software.

 

I’m particularly impressed with their Pages3D Professional product which combines illustration capabilities, using an embedded Solid Edge 3D model, with a powerful text editor for easy and rapid creation of technical documents. The added bonus is that your technical writers do not need a seat of Solid Edge to utilize the Solid Edge model. They just import the Solid Edge model, with its metadata, and they have the capability to rotate the model, create multiple views, create exploded views, section views and parts lists. You can even capture a technical document format into a custom template, allowing for rapid generation of documents, whose only difference is the model itself.

 

Users will have the ability to easily produce:

 

3D Work Instructions - Create work instructions packets and deliver to the shop floor. Includes support for printed, interactive 3D document authoring.

 

Illustrated Parts Catalogs - Design multiple-page illustrated parts catalogs complete with parts lists, balloons, exploded views, text, tables, images and 3D models.

 

Other Product Documents - Easily produce product manuals, service documentation, field instructions, inspection procedures, marketing materials and more.

 

Furthermore, these documents can be printed or delivered as interactive 3D documents. You can view 3D PDF documents with Adobe Reader, without plugins.

 

Never being one to trust the marketing material, I had to try it out for myself. I viewed the training material provide to me from QuadriSpace. I’ll be honest, I’ve seen better training material, but this is something that we can improve upon for our customer base. After going over the training material I opened the Pages3D and was able to easily import one of my Solid Edge training assemblies. Within minutes I was able to create an exploded view and generate an interactive parts list, as shown below.

 


 

Although I am not yet an expert, I’m very impressed with the ease at which customers will be able to utilize existing CAD models to rapidly generate all kinds of related documents. If you have to generate any technical documents for your CAD models, this package is worth a look. It’s relatively easy to learn, it’s easy to use, and it’s affordable. The most expensive single seat module is less than half the price of a seat of Solid Edge Foundation.

 

Designfusion has been so impressed with this software; we have become an authorized reseller for QuadriSpace. So if you would like to learn more, or would like to see a demo, contact your Account Rep. or contact us 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.  

Solid Edge: A baker’s dozen of Tips and Tricks (Part 3 of 3)

John Pearson - Friday, August 07, 2015

 

  • 9.Configurations for draft
  •  

Much like you create a configuration for your exploded view, you can create configurations for later use in your draft views. To do this you need to first turn off all the components that you wish to exclude from the view. Then create a new configuration of the components you want to show in the draft view. To do this, select the configuration command:

 


 

Click on the New button.

 


 

Enter in the name of this new configuration.

 


 

You can later place this named configuration as a separate view onto a draft sheet.

 

  • 10.Placing configurations in Draft
  •  

When placing an assembly into a draft sheet, using the Drawing View Wizard, you can select from a list of configurations or zones.

 


 

Only the components in that configuration will be visible in the draft view.

 

Note:If you wish to create a parts list of this configuration, you can set the Part List to only show the configuration components. To do this, open the properties of the Parts List and go to the List Control tab. Notice the Configuration option half way down the right side. Expand this and select the desired configuration.

 


 

  • 11.Placing section views in Draft
  •  

To place an assembly section view into a draft view, you must first place the assembly into the view. You then right click on to view and go to the view properties. On the Section tab you will find a list of all the assembly section views. Simply select the desired section view and then update the views to convert the assembly view into the section view.

 


 

  • 12.Drawing View Depth
  •  

By specifying a drawing view display depth for a back clipping plane, you can simplify any type of drawing view so that geometry behind the plane is removed from the view. This feature can be used, for example, to reduce the visible clutter behind a section view or a broken-out section view.

 

The Set Drawing View Depth command is found on the shortcut menu when you RMB click on the view.

 


 

You can type in a back clipping plane depth or use the companion view to set a depth.

 


 

You can remove the drawing view depth by using the Remove defined Depth command on the shortcut menu.

 

  • 13.Dimension Automatic Arrangement

 

Use the Arrange Dimensions command to automatically group, select, and arrange linear dimensions so they don’t overlap drawing view geometry and annotations.

 


 

There are three different ways to arrange dimensions;


  • I.Select a dimension

 


 

  • II.Fence select – drag a fence around the dimensions

 


 

  • III.Select a drawing view will select all dimensions for that view.

 


 

Note:This automatic arrangement command now makes it easy for you to use the Retrieve Dimensions command and quickly arrange the retrieved dimensions.

Thus ends our baker’s dozen tips and tricks. If all or most of these are new to you, consider upgrading your skills by attending one of our training courses. Here’s the link to the standard courses we offer; http://www.designfusion.ca//technical-training.html. We can also arrange custom training to meet your company’s needs. For more information contact your Account Rep or contact us 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.



Solid Edge: A baker’s dozen of Tips and Tricks (Part 2 of 3)

John Pearson - Tuesday, July 21, 2015

 

  • 5.Direct editing tool in the ordered paradigm.
  •  

The direct editing commands in Solid Edge allow you to modify models imported from other applications that do not have a feature tree, or to modify native Solid Edge design models without accessing the current feature tree.

 

 

 

Notice that in the Move Faces, Offset faces, and Rotate Faces, there is a select option to select the body.

 

 

 

This allows you to move, offset, or rotate the entire body.


  • 6.Flash Fit, for bolts and screws
  •  

When using the FlashFit option to place assembly relationships, you can select the bottom cylindrical edge of the bolt head and the top cylindrical edge of the hole to fully position the fastener, like the insert relationship.

 

     

 

Resultant relationships are Mate and Axial Align with rotation locked.

  


 

Note: To select the cylindrical edges you have to have the Circular Edges option turned on in the Assembly Relationship options.

 

 

 

  • 7.Capture Fit
  •  

Ideal for hardware or commonly used components, capture fit remembers what relationships and geometry you used to originally place your component. When you place the component again it will prompt you only for the target geometry.

 

To use capture fit you must first place the component into an assembly using the assembly relationships that you plan to capture. Then select the Capture Fit command and save the relationships in the dialog.

 

 

 

  • 8.Section views in assemblies
  •  

In the assembly environment, the Section command is found on the PMI tab.

 

 

 

The steps are similar to constructing a cutout feature for a part.

 

•Plane Step

•Draw Profile Step

•Side Step

•Extent Step

•Select Parts Step

 

For the last step you have options on how to determine which parts are to be sectioned.

 

 

 

When you are finished, you are left with a visual section view.

 

 

 

Note:You can hide and show the section view by toggling it on and off in the PathFinder.

 

 


Solid Edge: A baker’s dozen of Tips and Tricks (Part 1 of 3)

John Pearson - Thursday, July 02, 2015

 

Recently Designfusion held their annual Productivity Summit at the Microsoft office, in Mississauga. As part of the summit I presented a “Tips and Tricks” session that was well received. I promised that I would share these in a future blog article. So here is a baker’s dozen of tips and tricks:


    • 1.Holding down the Shift Key when using the Rectangle by Center command will create a square. (Added in ST7)

 

 

 

  • 2.Auto dimensioning done the correct way.
  •  

The biggest complaint with auto dimensioning is “I have to delete more dimensions than I would normally place”. However, if you use these settings Solid Edge will only place keyed in dimensions.


 


  •  
  • 3.Controlling rotation point
  •  
  • In the Select mode, Middle Mouse Button (MMB) click, in an empty screen space, to clear the small white select symbol attached to the cursor. The cursor will now appear with no symbols attached.

 

 

 

  • Move the cursor to one of the following positions and hold down the MMB to rotate:
  •  
  • I.Hold the MMB down on a vertex to rotate about the vertex.

 

 

 

  • II.Hold the MMB down on a linear edge to rotate about the linear edge.

 

 

 

  • III.Hold the MMB down on a face to rotate about the point on a face.

 

 

 

  • IV.Hold the MMB down on a circular arc or conic-shaped edge to rotate about the axis of the circular arc or conic-shaped edge.

 

 

 

  • 4.Clipping planes
  •  

I.Choose View tab→Clip group→Set Planes.

 

 

 

II.Select a planar face or reference plane, position the cursor to define the first clipping plane (A), and then click.


III.Position the cursor to define the second clipping plane (B), and then click.

 

 

 

IV.Click Finish.

 

 

 

Note: When you set the Dynamic Clipping option on the command bar, the clipping depth updates dynamically as you move the cursor during the Set Plane 2 Step. When you clear the Dynamic Clipping option the clipping depth updates when you click to define the second clipping plane.


Note: You can turn the clipped display on and off using the ‘Clipping On’ command, located below the Set Planes command, or use the Hot Keys (Ctrl + D).