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How to Find the Volume Capacity of Container

John Pearson - Thursday, January 28, 2016

It is sometimes necessary to determine the volume of a container. This is a relatively easy process to do, if you understand a few simple surfacing commands. For this article I will use the Hopper pictured below.

 


 

In this example I need to know the volume of sand that this hopper can hold. To determine this, I need to create a construction volume of the inside of the assembly. For this to work efficiently I need to know that the assembly is assembled correctly. In other words, I don’t want any gaps between the seams or joints of the hopper. Once I’m sure that this is true, I use the Create in Place command to create a part within the assembly. I give the part a name like Volume1.prt. The command then places me inside the Volume1.prt with the underlying assembly components visible, but dimmed.

 


 

Next I use the Inter-Part Copy command and I get all the inner faces of each part in the assembly.

 


 

For example, the Inter-Part Copy command prompts me to pick a part to copy from, so I select the back part, as shown.

 


 

I’m then prompted to select what I want to copy. I set the selection filter to Face and select the inside face of the part.

 


 

I accept this selection and I am left with the inside face construction surface.

 


 

I then repeat these steps for all of the components in the assembly. Once completed, I hide the assembly components by using the Hide Previous Level command. This is found on the View tab, in the Show group. I am left with all the inside faces of the hopper.

 



 

Note: If your assembly components are aligned properly these faces can be capped and stitched into a solid. Poor alignment may leave gaps and require more work to stitch the surfaces together.

 

Next I will use the Bounded command, from the Surfacing tab, to create end caps on this surface model.

 


 

I select the four top edges to form a closed loop and accept them to create a flat surface at the top.

 


 

I then repeat this step to create a bounded surface on the bottom. Note, the order in which I create the surfaces is not important, but I must have all the surfaces created before proceeding to the next step.

 


 

To turn this into a solid, I will use the Stitched command, found on the Surfacing tab.

 


 

I accept the defaults when the Stitched Surface Options dialog appears and hit OK.

 


 

I select all the surfaces and click Preview.

 


 

If I have aligned my components, and extracted the correct surfaces, I should receive this message.

 


 

I hit OK, and I’m left with a solid body representing the inside of the hopper.

 


 

To find the volume, of this solid body, I go to the Inspect tab and click on the Physical Properties command.

 


 

When the dialog appears, I make sure to click on the Update button, at the bottom. Since I haven’t assigned a material, I get this warning message.

 


 

Since I don’t care about the mass of the solid, I hit OK and the system gives me the volume of the solid.

 


 

I now have the capacity volume of this hopper. I can save this part with the assembly, but have it not appear in the draft files, or bill of materials, by setting omission options in the occurrence properties.

 

If techniques shown in this blog are unknown to you, I suggest you attend some of our advanced courses. Surfacing is taught in the Advanced Modeling course and Physical Properties and occurrence properties are taught in the Advanced Assembly course. For more information visit our website at http://www.designfusion.ca//technical-training.html or contact us at info@designfusion.com.

 


The right tool for the right job (part 2)

Dominic Benoit - Tuesday, January 26, 2016

In the first part of the article “The right tool for the right job”, I started illustrating one of the aspects where the drawing and the programming software reach each other. In the following, I’ll point out some other elements that belong to each application type.

 

Once opened in the Drafter application of act/cut, the drawing can be modified, corrected and rotated by the user in order to match the horizontal orientation of the part with the horizontal direction of the plate. It’s particularly useful for the parts with brushed finish or that will be cut in a plate with a pattern. If it contains doubled or overlapped lines those will be eliminated and if the endpoints are not connected, it will become apparent.

 


 

Fig. 3- act/cut shows a red X where the contour is not closed.

 

For a subcontracting company who receives all sorts of drawings, it is essential to be able to make the necessary corrections to ensure manufacturability of the parts and avoid returning the drawings to the sender to offer faster delivery. The tools are in place in the Drafter of act/cut to repair typical imperfections.

 

For a continuous cutting technology, act/cut will determine a cutting direction according to the machining operation (left or right kerf compensation). To achieve this, the external contour of the piece must form a continuous chain. Solid Edge meanwhile provides no indication of the direction of the profile chain. This information is required especially for the continuous cutting technology.

 

On a counterpart, the Solid Edge user can determine the orientation of the flat pattern when he uses the Flatten command. Solid Edge will output a clean geometry, without doubled or overlapped lines nor disconnected junctions.

 

After orienting the part in act/cut, the programmer can decide to authorize the part to be rotated in the nest to improve part placement or prevent it from rotating to respect the grain direction of the sheet.

 


 

Fig. 4- Nesting authorization settings in act/cut.

 

For better cutting finish, some machine can adjust their speed based on the size of the contour to cut (diameter or perimeter), it means that each contour within a part will be using different cutting parameters. For that reason, the act/cut user must use auto-tool allocation to apply proper parameter to each contour.

 


 

Fig. 5- The colors indicate that act/cut recognized the machining parameters according to the size of the contours.

 

After the parts are all prepared, they will be regrouped per material/thickness in a Launching order in which one can specify the quantity of each part to produce and also the selection of sheet size available to nest. Following this, the optimal toolpath is generated and the nc program is being written for the complete nest.

 

As you may notice, whether in the drawing or in the programming software, a lot of tools exist to ensure a good integration of the various platforms with each their speciality. Should you be a manufacturer with your own cutting machine or you outsource the task, being aware of the parameters and the needs of each other’s platform will help streamline the exchange process.

 


The right tool for the right job (part 1)

Dominic Benoit - Tuesday, January 19, 2016

Often times we are being asked: “Can Solid Edge do the programming for the machine that is going to produce the parts? ” My answer always comes to the principle that every pieces of software has its speciality. For example, when it concerns sheet metal parts, it will be cut on a continuous cutting technology (Laser, plasma, milling) or on a punching machine. As we can assume, each type of machine has in strength. Some technologies are better for thick material while others are very fast on thin parts. Some have a large size stationary table; other like the punching machines have a moving table and other can only hold one piece at a time. Here I refer to wood panel machining center with a wide array of tool type (saws, drills, mills and even label printer) and can machine on several faces of a part. This quick overview is just illustrating the range of specialisation that is involved when we think of programming a part to produce.

 

Solid Edge is an engineering and drawing platform. Programming software is essential in the preparation (offline) of the programs that will run on the machine. Moreover, all machines don’t “speak” the exact same language, even though the G-Code format is standard, taking into account of the level of instruction that the machine manufacturer put in the head (the controller) of the machine. So, every time that a software writes a program for a specific machine, it has to know what instructions the machine is expecting, how it’s expecting it and also, which ones don’t need to be given. This task belongs to the post-processor that goes with the programming software.

 

At the drawing stand point, there is no way we can specify that much information precisely for the manufacturing technique. So, outputting the outer and inner contours of the geometry that need to be cut or engraved is enough. Another article on our blog explains how to use the command that prepares the drawing for manufacturing a sheet metal part (How to save a flat pattern as a .dxf file in Solid Edge).

 

Programming applications all have their level of comprehensiveness of the programming needs particularly if they are developed by a machine manufacturer or by an independent software editor.

 

The programming software that I’m talking about in my article is act/cut, edited by a French company Alma, it is independent of any machine manufacturer. Act/cut’s strength is in its ability to be adapted to communicate with various types of machines within the same environment and in its calculation algorithms for nesting parts.

 

The most common exchange format for manufacturing drawing is of course .dxf. That’s why it seems logic for Solid Edge to export in this type with the command Save as flat. It’s also logical for act/cut to import this format smoothly. Act/cut can also import native CAD files from well-known software thanks to an add-on module.

 

When a .dxf is opened of the Drafter application of act/cut, a filter can be used either by Layer, by color or both Layer/color. This filter allows eliminating undesired elements up-front. For example, 2D drawings often have some dimensions on a specific layer, we don’t want to cut those as part of the piece, and then we remove them right away.

 


 

Fig. 1- Layers filters in act/cut.

 

Some parameters can be setup in act/cut’s resources to indicate in advance which layer or color must be excluded or included and what type of contour are they representing. Does it represent geometry to cut or to engrave or even is construction or cosmetic? This leads to enable batch import of files.

 

For its part, Solid Edge also provides parameters to control layer filtering in the Save as flat command. Once set, these parameters are stored in order to prevent from having to redefine them again each time.

 


 

Fig. 2- Layer filters in Solid Edge.

 

Many other aspects are to be considered in determining what role is played by which software regarding parts fabrication. I’ll cover more in an upcoming article.

 


Moving or Renaming a Subassembly with Revision Manager

John Pearson - Friday, December 18, 2015

For those of you that use revision manager, this may be a non-issue, but some users still have an issue with intelligently moving or renaming subassemblies or parts. So at the risk of over simplifying the issue, I’ve put together a simple example to illustrate how to achieve this task.

 

The scenario: I have created a Test folder representing my server. Inside this folder there are 5 other folders as shown below:

 


 

Folder1, Folder2, and Folder3 each contain a different assembly. These 3 assemblies all use a subassembly that currently resides in the OLD folder. The goal is to move and rename the subassembly from the OLD folder to the New folder, without breaking the links to the 3 assemblies in Folder1, Folder2, and Folder3.

 

To start the process, I open the OLD folder, locate the subassembly, and RMB click on it to select “Open with Revision Manager”.

 


 

Note: I could also open the View and Markup program from the Start Programs menu and then open the file in Revision Manager, from View and Markup.

 


 
 

 

Once in Revision Manager, I highlight the subassembly and its components as shown below.

 


 

Note: If you click on the top left grey square, it will highlight all the occupied rows below it.

 


 

Next, I go to the Tools tab and select the Where Used command, in the Assistants group.

 


 

The Where Used dialog appears and allows me to set up my search scope. In this example, I want to search the TEST folder in my C drive. Notice that I have also toggled on the Include subfolders option, near the bottom of the dialog.

 


 

Note: Under the Process options button, I could filter the type of files that I am searching.

 

Once my search scope is set up, I click Next. The process runs and reports back to me the Number of documents processed: and the Number of documents found:

 


 

I click Finish, to dismiss the dialog. I am left with a list of where the subassembly and its components are used. Remember this list is only based on my search scope. If the subassembly or its components are used outside of my TEST folder, it will not show up unless I expand my search scope.

 


 

Now I will move and rename my subassembly. To do this I RMB click over the highlighted components and select Set Action to Rename.

 


 

Note: I could also click on the Rename command on the home tab, in the Action group.

 

Notice the New Filename column becomes populated.

 


 

I now either click on the Set Path command, on the Home tab > Action group, or RMB click and select Set Path from the shortcut menu. This launches a browse dialog. From there I select the New folder, which is the location that I want to move the subassembly and its components.

 


 

When I click OK, the New Filename column is updated to the new path.

 


 

Now I can rename the components. In this case, I want to replace the “exp” prefix with a “new: prefix. To do this I select the Replace command from the Home tab>Edit group.

 


 

I set the dialog up to find and replace “exp” with “new”, as shown below.

 


 

Once I completed this process I see the new names, along with the new location, listed in the New Filename column.

 


 

These changes have also occurred in the Where Used section of the Revision Manager.

 


 

Before I tell the system to make these changes, I need to tell it to update all the parent assemblies that use this subassembly and its components. To do this I first highlight all the listed parent assemblies, as shown below.

 


 

Next I either click on the Update command on the Home tab>Action group, or I RMB click and select Set Action to Update from the shortcut menu. This populates the New Filename column in the Where Used section as shown below.

 


 

Now I simply review all my actions and once satisfied I click the Perform Actions command.

 


 

Once the process is complete, I can exit the Revision Manager, and confirm my changes. I confirm that my OLD folder is now empty and that my New folder is populated with the newly named subassembly and its components.

 


 

I can open the assemblies in Solid Edge or Revision Manager to confirm that there are no broken links.

 

Although this was a simple example, you can see how this can be used on a larger scale. Revision Manager is a powerful and reliable tool that helps you manage your data in a non-managed environment. If your data has become too large to easily manage you should consider implementing Teamcenter.

 

Teamcenter is the world's most widely used PLM solution. For manufacturing companies who need to deliver increasingly complex products while maximizing productivity and streamlining global operations, Teamcenter helps increase revenue, get to market faster, reduce costs and improve product quality. Teamcenter simplifies PLM with targeted applications available to do what customers need when they need it. Platform capabilities get customers up and running quickly with a high definition user experience to inform decision-making anytime, anywhere. Applications are built on the PLM platform to help customers grow their deployment strategically over time.

 

For more information on Teamcenter, please visit our website at http://www.designfusion.ca//teamcenter.html or contact us at info@designfusion.com

 


How to: Reverse Engineer a Feature from a Round Surface

Manny Marquez - Tuesday, December 08, 2015

 

More videos here: https://www.youtube.com/EdgeCanada


How to Search the Assembly Pathfinder for a Named Component

John Pearson - Wednesday, November 18, 2015

Solid Edge has a nice tool that can save you a lot of time if you need to isolate specific named parts in a large assembly. This tool is called Quick Query and can be found on the Select Tools tab of the PathFinder.

 


 

Let’s assume that you have to locate a component in a very large assembly. All you have is the component’s name to go by. Here are the steps to use the Quick Query to locate the named component.

 

  •    1.On the Select Tools tab, position your cursor over the Quick Query box, then right-click to display the shortcut menu.

 


 

   2.On the shortcut menu, set the Property option you want. In this example you need to select the Name property.

 


 

   3.On the shortcut menu, set the Condition option you want. You can set the condition to Contains, Is (Exactly), or Is Not.

 


 

   4.On the shortcut menu, click the Scope button to display the Scope dialog box, and then set the scope options you want.

 

 


Note: Solid Edge will remember the settings, so you only have to set them once if you continue to use the same property, condition and scope settings.

  

   5.On the Select Tools tab, type the value property you are searching for in the Quick Query box, and then click the Go button.

 


 

The parts that match the query properties you’ve defined are selected in the assembly window and PathFinder.

 


 

 

Note:Since the condition was set to Contains, it was not necessary to include the file extension. In fact, you do not even have to type the full name.

 

In this example, the Name property was used, but one could also search for components using any of the other properties listed in the quick query shortcut menu.

 

Quick queries are not stored on the Select Tools tab. If you wish to create a permanent query, click on the New Query button, on the Select Tools tab.

 

 

 

The Query dialog box will appear. Here you can define the query scope and criteria, as above, but you can also give the query a name. For example, below is a query, called Conveyor, which searches for the Category property which contains the word Conveyor.

 


 

Using this method saves the query in the assembly file for future reuse.

 


 

Queries can also be saved in the assembly template, so they can be reused in any of your assembly files, created from that template.

However you choose to use the queries they will provide quick and accurate search capabilities within your company’s assembly files.

 


How to Manage Dimensions in Draft Part 4

Manny Marquez - Thursday, November 05, 2015


Part 1: https://www.youtube.com/watch?v=d3pXCcPMin4

Part 2: https://www.youtube.com/watch?v=nVAmo2xrVd0

Part 3: https://www.youtube.com/watch?v=2jQKqw0urCk

 

More videos here: https://www.youtube.com/EdgeCanada

 





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.