Posts Tagged ‘Synchronous Technology’

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Simplifying the placement of certain dimensions in Draft

Tuesday, April 17th, 2012support

Recently I had a customer contact our support line, looking for an easier way to place some dimensions. He was self taught on Solid Edge and was attempting to place the following dimensions on a formed tube.

 

 He had figured out how to do this by creating and using extra sketches, but felt there should be an easier way to achieve his desired results. I walked him through the process, and felt that this would be a good tech tip to share.

To place the 2 dimension shown, do the following:

1. On the Sketching tab, in the IntelliSketch group, make sure that the intersection option is toggled on.

 

2. From the Home tab, in the Dimension group, select the Distance Between command.

 

  •  
    • - Make sure your option is set to Horizontal/Vertical on the command bar.

 

  •  
    • - Move the cursor over the bottom centerline so it highlights. DO NOT CLICK

 

  •  
    • - Now move the cursor over the angled centerline and hit the ‘I key’ on your keyboard. (I is for intersection)

 

  •  
    •  - Then move the cursor over to the vertical centerline and click.

 

  •  
    • - place the dimension.

 

Note: Hitting the ‘I key’, tells the system to find and select the intersection point between the 2 highlighted lines. If more than one intersection point is possible, a list window will appear allowing you to select the desired intersection point.

3. From the Home tab, in the Dimension group, select the Angle Between command.

 

  •  
    • - Make sure your option is set to Horizontal/Vertical on the command bar.

 

  •  
    • - Select the horizontal centerline at a non-keypoint.

 

  •  
    •  - Select the vertical centerline at a non-keypoint.

 

  •  
    • - Place the dimension.

 

Note: the trick here is to not select the lines at keypoints (endpoints or midpoints).

There are several hot keys and various command options, which assist in placing dimensions in sketches and draft files. Take the time to review the help section on each dimension command and you will save yourself a lot of time and frustration.

Is Training Worth It? – Calculate your Return On Investment

Tuesday, March 27th, 2012partner

In today’s competitive market, businesses are looking to get the most out of their employees, systems, software and machines. With the ever changing technology, this can be somewhat challenging.  Too often companies will invest in new technology but not invest in the training on the new technology. The most common reasons for this are:

  • - I don’t have the time to take the training.
  • - I can’t afford the cost of the training.
  • - I can train myself for free.
  • - I train one employee and he/she can train the rest.
  • - I have a high staff turn over and it’s not worth training them.

As a trainer I have heard all these excuses and more. They all essentially evolve around cost. Therefore, it is important that companies look at both the ROI of professional training and the cost of not taking professional training.

How to calculate the ROI of professional training

To calculate the ROI, you need to determine the total cost of the training course and compare it to the total financial benefit derived from the course. The cost of the course can be determined as shown below:

Cost of course                   = $ 2000

Salary of employee           =  $1000

Travel & Living Expenses  = $1000

Total cost of course           = $4000

The financial benefit derived from the course can be a little harder to determine and often depends on the individual. Below is a one potential example;

Suppose John Smith attends a course on a CAM software package. In this course he learns new and faster methods to create programs. Assuming a modest 10% increase in his program generation skills, we can start calculating the financial benefit. If John makes $25 per hour and he works 50 weeks a year week, allowing 2 weeks for vacation, the company pays him $50,000. If he works 10% faster the company’s immediate savings is 50,000 x 0.10 = $5000. We can also assume that John’s programs will be more efficient, saving machine time, cutter wear, and possibly less manual finishing work. His improved knowledge may also lead to fewer errors in the programs, resulting in less scrap. You may also want to consider any extra profits obtained by the increase efficiency. In other words John will be able to produce 10% more work from which the company will profit. So in John’s example we can calculate the financial benefit as follows:

Estimated savings from improved output                     = $ 5000

Estimated savings from downstream operations         = $ 2000

Estimated savings from reduced rework and scrap   = $ 1000

Estimated additional profit from improved efficiency    = $ 2500

Total financial benefit                                  = $ 10500

Using the following formula to calculate the ROI,

Net gain (total benefit-total costs) = ____ X 100 =____
  total costs  

we get an ROI of 162.5. Clearly this would justify John taking the course, especially when you consider that the financial benefit estimates are very conservative.

You can also view this from another direction. What is the company’s cost if an employee doesn’t take professional training?

Cost of not taking training

Let’s assume that you hire a new designer. This designer has CAD experience but does not know your CAD system. You hand him\her a manual or some tutorials and have him\her learn the system on their own. From the previous example we can assume that you are saving $4000 dollars in training. But how much are you really saving?

Although estimates vary on the topic of study, many agree that 1 hour of professional training could be equal to as many as 16 hours of teaching yourself. In other words you could spend up to 2 days reading, experimenting and learning a process that a professional trainer could teach you in 1 hour. If we extend this model we have one week of professional training = 16 weeks of self teaching. The cost to the company at $25 per hour is:

640 hours (16 weeks) x $25  =  $16,000

You also have to factor in the lost time in production for 15 of those 16 weeks that the new designer is not producing because the are still trying to learn the software. Any mistakes made through this process will also have a ripple effect throughout the company, costing more time and money. You also have to consider lost production time from any experienced employees who may be mentoring the new employee. If the experienced employee spends an average of 20% of his time helping the new employee you will lose one full week of man hours in every 5 weeks.

So for a conservative estimate, let’s assume that a new employee can learn the CAD package in 10 weeks with some assistance from experienced employees. Each week the new employee improves his/her output by 10% per week. The cost to the company can be calculated as follows:

Cost of no productive work over 10 weeks is:

  New Employee Experienced Employee
Week 1 1000 200
Week 2 900 200
Week 3 800 200
Week 4 700 200
Week 5 600 200
Week 6 500 200
Week 7 400 200
Week 8 300 200
Week 9 200 200
Week 10 100 200

Total cost of lost production  =     5500  +  2000 

                                                  =     7500 

Remember you still have to factor in the cost of fixing any training errors and the downstream effect of each error. If we assume a modest 5 errors, at an average cost of $500 per error, this results in:

Total cost of lost production = 10,000

Keep in mind that the cost could be much higher depending on the new employee’s ability to teach him/her self, and how many errors are made in the process.

Finally, you’ll have to wonder if the self taught employee has learnt the most efficient use of the software. With today’s software there are often several methods to achieve the same desired results. Each method has advantages and disadvantages depending on downstream factors. Too often self taught individuals find one method to solve a problem and use it, without further investigation to see if a more efficient way exists.  A good professional trainer will teach the different methods highlighting the situations where each method is most efficient.

Other excuses

Some companies have chosen to train one employee and have him/her train the others. They look at this as a cost savings to the company. Although this may appear to save you money you have to factor in the cost of using the first employee as your trainer. Every time he/she is training other employees, he/she is not producing work. Plus the assumption is being made that this employee has learned and retained the same knowledge as the professional trainer. This is often a false assumption, leaving the company paying almost a similar cost for a lower standard of training.

I’ve saved my favorite excuse for last. Some companies will not pay for professional training because they have too high of a staff turn around. It has been proven time and again that stress levels rise in adults when they have to learn something new. If you combine the stress for self teaching with the daily stress of the workplace, you may be contributing to the staff turn around. By providing professional training in a setting designed for learning, the employee will learn, without the work stress, and return to work with the proper skills.

Conclusion

When you actually take the time to do an honest, realistic cost analysis, it quickly becomes clear that sending your employees for professional training is a good investment.  The above examples are very conservative, yet they clearly show the advantage to professionally training your staff. Although it may be difficult to free up time and money to provide professional training, the cost of not doing so will be greater in the long term.

A well-trained employee is more likely to be satisfied with the company he\she works for, which in many cases means he\she will be less likely to leave to find a job elsewhere.  The payback is not just in a few months or a year. Instead, it can be a lifetime of service and reduced operating costs.

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Non-graphic parts in Solid Edge assemblies

Friday, March 9th, 2012

Assemblies often contain components for which there is no model required, such as paint, grease, oil, labels, and so forth. These non-graphic parts still need to be documented in the parts list and bill of materials that are created for the assembly. In Solid Edge, you can use the File Properties command on the Application menu in the Part and Sheet Metal environments to add custom properties to an empty part document. These custom properties allow you to define the required information for these types of parts. You can create two types of non-graphic parts: parts that require a unit type and quantity, and parts without a unit type and quantity.

 Types of non-graphic parts

Parts with a unit type and quantity

Some non-graphic parts require a unit type and quantity. For example, you may require four liters of oil in an engine assembly. You can create a part document named OIL.PAR, and then set the unit type, Liters, in the part document. Later, when you place the oil.par document in the assembly, you can set the unit quantity using the Occurrence Properties command on the Edit menu.

Parts without a unit type or quantity

Other non-graphic parts require no unit type or quantity. For example, you may require a small quantity of grease between certain parts in the assembly. These types of part quantities are usually documented “As Required” on a parts list or bill of materials. For these types of parts, you define the custom properties and the text string you want in the part document. You do not have to edit the occurrence properties in the assembly.

 Placing Non-Graphic Parts

Since non-graphic parts do not need to be positioned with assembly relationships, you can place the part in the assembly by holding the SHIFT key, and drag the part into the assembly.

 

Create a non-graphic part that uses units and value

This procedure shows you how to define custom properties for a non-graphic part that requires units, and a value for those units. Although no 3D model is required for these parts, they still need to be documented in a bill of materials or parts list. For example, you may require 4 liters of oil in an assembly.

Step 1. In the part document, choose Application menu→Properties→File Properties to open the Properties dialog box.
Step 2. On the Custom tab, in the Name box, type: SE_ASSEMBLY_QUANTITY_OVERRIDE.
Step 3. In the Type box, select Number from the list.
Step 4. In the Value box, type 0 (zero). Then click the Add button.                                                                                                                                 
Step 5. In the Name box, type: SE_ASSEMBLY_QUANTITY_STRING.
Step 6. In the Type box, select Text from the list.
Step 7. In the Value box, type the unit and number of decimal places you want. For example, Liters;4. Then click the Add button.           

Note:  You must separate the unit type and decimal places with a semi-colon (;). If the number of decimal places you want is 2, you do not need to enter a value for the decimal places.

To use the custom properties in an assembly, do the following:

Step 1. Place the part in the assembly.
Step 2. Select the part in the PathFinder tab or the graphics window, then on the shortcut menu, choose Occurrence Properties.
Step 3. On the Occurrence Properties dialog box, type the quantity value in the Quantity cell for the occurrence. Notice that the unit value you specified in the part document is displayed in the User-Defined Quantity column.

Tip:

  • - You can place a non-graphic part in an assembly without applying relationships by holding the SHIFT key, then dragging the part into the assembly.
  • - You can also set the quantity value using the Occurrence Properties button on the Place Part command bar.
  • - If you use many non-graphic parts at your company, you can create a template that has the non-graphic part custom properties defined.

 

Create a non-graphic part that is unit less

This procedure shows you how to define custom properties for a non-graphic part that does not require units. Although no 3D model is required for these parts, they still need to be documented in a bill of material or parts list. For example, you may require a small quantity of grease that on the parts list is documented “As Required”.

Step 1. In the part document, choose Application menu→Properties→File Properties to open the Properties dialog box.
Step 2. On the Custom tab, in the Name box, type: SE_ASSEMBLY_QUANTITY_OVERRIDE.
Step 3. In the Type box, select Number from the list.
Step 4. In the Value box, type 1 (one). Then click the Add button.                 
Step 5. In the Name box, type: SE_ASSEMBLY_QUANTITY_STRING.
Step 6. In the Type box, select Text from the list.
Step 7. In the Value box, type the constant text you want. For example: As Required. Then click the Add button.                                                       

 

To use the custom properties in an assembly, do the following:

  • - Place the part into the assembly. The “As Required” property is automatically recognized in the Occurrence Properties dialog box. To review the part’s properties, select the part in the PathFinder tab or the graphics window, then on the shortcut menu, choose Occurrence Properties.

Tip:

  • - You can place a non-graphic part in an assembly without applying relationships by holding the Shift key, then dragging the part into the assembly.
  • - If you use many non-graphic parts at your company, you can create a template that has the non-graphic part custom properties defined.

 

Set part properties in an assembly

  1.  Click a part or subassembly in the assembly.
  2.  Right-click, then choose Occurrence Properties on the shortcut menu.
  3.  In the Occurrence Properties dialog box, set the options you want to use.

 Tip:

  • - You can also set the part properties with the Occurrence Properties command on the shortcut menu when a part or subassembly is selected.
  • - When you select the top level assembly entry in PathFinder, then click the Occurrence Properties command, the entire assembly structure is displayed in a bill of materials format. You can use the (+) and (-) symbols to expand and collapse the assembly structure.
  • - When you select one or more parts or subassemblies, the selected occurrences are displayed in a table format that cannot be expanded or collapsed.
  • - If you need to change the properties of a subassembly, you must first check out all subassemblies where the occurrence properties are being modified. Then the documents can be saved and checked back in to Teamcenter.

*Text passages taken from Solid Edge Help files.

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New Parts List Architecture

Tuesday, January 17th, 2012support

In Solid Edge ST2, Parts Lists were redesigned to take advantage of the user table architecture. The new architecture was needed to meet the demands of our customers. In this first release of this new Parts List command, just under 250 customer requests were implemented, and many more have been added in ST3 and ST4. Below is a list of highlights followed by some example of the new capabilities.

 Highlights

 The new Parts List architecture allows you to:

  • - Edit Item Numbers from Parts List, not just from balloons
  • - Combine Multiple Properties in Single Column
  • - Comments Columns – User defined text
  • - Split Parts List among Multiple Sheets
  • - Sort on Hidden Columns
  • - Manual Reorder Columns and Rows
  • - Resize Columns in Graphic Display
  • - Placement via cursor
  • - Title/Footer
  • - Display an exploded list of the BOM
  • - Display level based item numbers with the exploded list
  • - Indent any column to aid in the showing of sub-assemblies
  • - Derive item number from the assembly
  • - Display Mass property as Mass of single item, and Mass of total occurrences of the item
  • - Frame data display enhanced to allow for distinction of frames based on cut length, mass, and miter
  • - Align and control style of table titles
  • - Control column headers
  • - Merge column headers
  • - Rotate column headers
  • - Turn on Cell Aspect Ratio adjustment
  • - Format the font for any cell
  • - Override disabled cells
  • - Insert user defined rows
  • - Merge vertical cells with same value
  • - Plus more ….

 

Examples

The following are just a few examples of some of the new capabilities in the new Parts List architecture.

 

 

Example 1: How to add a title to the Parts List

 To add a title to your Parts List you must first go to the “Title” tab and click on the Add Title icon.

In the Title text field, type the title that you wish to use – for example Solid Edge Parts List.

 You can also control how the title is formatted by adjusting the following settings:

Position – Specifies the position for the title within the table. You can place a title at the top of the table (Header option), at the bottom (Footer option), and in ‘Both’ locations.  Select ‘Neither’ from the list if you do not want to use the title in the table.

Font – Specifies the font to apply to the currently selected table title. All installed fonts are available.

 Font style – Specifies the font style to apply to the currently selected table title. The options are Regular, Bold, Italic, and Bold Italic.

 Font size – Specifies the text size of the currently selected table title.

 Alignment – Adjusts the horizontal alignment of the currently selected table title text. The options are Left, Center, and Right. The default is for text to be centered.

 Underline – Applies underline to the currently selected table title text.

 Adjust text to title width – When checked, automatically adjusts the aspect ratio of the title text when the length of the text exceeds the cell width. Changing the aspect ratio only changes the text width, not its height. The effect of selecting this check box is to shorten the text string to fit the column width; text is never lengthened to fit the column width.

Use this option to prevent text from wrapping within a cell in a title block.

For this example I set the following settings:

  • - Font = Arial Black
  • - Font size = 7.00mm
  • - Toggle on Underline

  

Below is how this would appear on my Parts List.

 

 

Example 2: How to modify individual columns

In this example I wish to rotate the header of the ‘Quantity’ column and merge any cells that have the same quantity, while maintaining my item number order. To do this I first go to the Columns tab, and select the Column that I wish to modify – for example ‘Quantity’.

To rotate the header, select the ‘Format Cells’ button, beneath the header ‘Text:’ field, and change the Orientation to Rotated

I then toggle on ‘Adjust text to column width’ and hit OK.

Notice that when this is applied, the header is rotated and column width is adjusted appropriately.

To merge like cells, toggle on “Merge vertical cells with same value”

If you wish to center the cell’s data, click the adjacent “Format Cells”  button and set both Horizontal and Vertical alignment to ‘Center’ and click OK.

Below is an example of how these changes would appear when applied.

 

 

Example 3: Creating indented item numbers

In this example I wish to create an exploded BOM and have the Item Numbers indented to illustrate the parts belonging to the sub-assemblies. To do this I select the Columns tab. Next I select the Item Number, from the Columns list, and click on the ‘Format Cells’ button. Under the Horizontal alignment I select Indent. 

  

Next I go to the List Control tab.

  

Here you will select the type of list you want, in this case an ‘Exploded list’. Under the Global settings, change the settings to match those shown below.

You can preview the results on the Data tab. Notice the indent item numbers for assembly number 1.

 

 

Summary

The new Parts List architecture has allowed the Solid Edge development team the ability to add a tremendous amount of user control to Parts List creation. For more information view the ‘Parts List’ section found in the Solid Edge Help documents.

New training schedule announced for the first half of 2012

Thursday, January 5th, 2012partner

If your New Year’s resolution is to improve your Solid Edge skills, then this is the article for you. We have released our new training schedule for the first half of 2012. The schedule includes some new course offerings, along with our traditional courses. Below is a brief description of each Solid Edge course along with a link to a more detailed outline.

Solid Edge Fundamentals (4 days) or Solid Edge Fundamentals Plus (5 days)

This is our introductory course for any novice user. The first four days cover both ordered and synchronous part modeling, assemblies, and drafting. The 5th day is optional and covers sheet metal modeling. For more information follow this link http://www.designfusion.ca/se_fundamental_plus.php.

Solid Edge ST4 Update Course (2 days)

This is our “What’s New in ST4 course”. It focuses on introducing the experienced user to the popular enhancements in our latest release of Solid Edge. For more information follow this link http://www.designfusion.ca/st4update.php.

Advanced Solid Edge Modeling (3 days)

This is one of our newer courses. It’s designed to improve the users’ modeling skills by introducing them to surface modeling, along with advanced modeling tools. Many of the techniques taught in this course have been included based upon queries we have received from our technical support line. For more information follow this link http://www.designfusion.ca/advancedmodelingcourse.php.

Advanced Solid Edge Assembly (3 days)

This course is for the more experienced user, who wants to improve his knowledge in working with assemblies. It focuses on improving the user’s assembly design skills and introduces many advanced assembly design tools. For more information follow this link http://www.designfusion.ca/advancedSEassemblyCourse.php.

Solid Edge Synchronous Technology Course (4 days)

This is our newest course, and is designed for our traditional users who have yet to learn the new synchronous paradigm. Its focus will be on showing the difference between ordered and synchronous modeling and how to use both paradigms to improve your design productivity. For more information follow this link http://www.designfusion.ca/synchronous_tech_course.php.

All of our courses are designed in house, by a certified trainer of adults, and are unique to Designfusion.

All of our instructors are SETA certified and come from a CAD/CAM industry background with many years of experience.

For our course schedule, please visit the following web sites:

English courses in Canada: http://www.designfusion.ca/training_schedule.php

French courses in Canada: http://www.designfusion.qc.ca/events.php

Courses in the USA: http://www.designfusion.com/training_schedule.php

For further inquires, including requests for quotes, please contact your local Account Manager. You can also contact the appropriate inside sales representative listed below:

English Canada:      Rose Francella at rfra...@designfusion.com

French Canada:       Lily Brault at lbra...@designfusion.com

USA:                           Sarah Pritsch at spri...@designfusion.com

Remember, it is estimated that 1 hour of an instructor led course is equivalent to 16 hours of teaching yourself. Students, who have attended our courses, see immediate benefits for themselves and their companies.

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Editing with Live Sections

Tuesday, December 13th, 2011

In the Solid Edge synchronous modeling paradigm, you can use the Live Section command to create a 2D cross-section on a plane through a 3D part.

Live sections can make it easier to visualize and edit certain types of parts, such as parts that contain revolved features. You can then edit the 2D elements of the live section to modify 3D model geometry.

Recently we have received some questions from customers who have received synchronous models, which they need to edit. They are still working in the ordered paradigm and have not taken any synchronous training. They want to know how they can accurately edit a synchronous part. For these customers, we often show them how to use the Live Section command. It is similar to working with dimensional sketches and is often easier to visualize than some of the other approaches. Below is such an example:

Scenario: The user has a synchronous roller part for a conveyor mechanism, as shown below.

 

The user wishes to edit the part to look like the following part.

First, it should be noted that there are several ways to edit this part. But we will illustrate a method using the Live Section command. To create a live section you follow these simple steps:

          1.  Choose Home tab→Section group→Live Section.

          2.  Select an existing planar face, reference plane, or principal plane on a coordinate system.

 

          The live section is created.

Tips:

  • - You can use the Live Section Colors section on the Colors page of the Solid Edge Options dialog box to specify the colors you want to use for the edges, center lines, and regions for live sections.
  • - You can use PathFinder to display and hide live sections.
  • - The live section automatically updates when you add or remove features, or modify the 3D model.
  • - Move the live section plane and the section updates as the plane intersects the model.

 

To get a better view of the live section, hide the design body using a RMB click over the display screen, to access the following menu:

Align the view to give you a top down view of the live section. Below is a list of keyboard shortcuts to help you orient your view.

In this case I used a Ctrl+R to get the top down view of the live section.

I then used the Distance Between command to place the following dimensions.

In this scenario, I have to modify the 1.000” to 0.500” and the 0.875” to 0.375”. I first select the 1.000 dimension. I ensure that the directional (red) arrow is pointing to the side that will move. I then type in the 0.500 value.

Before hitting enter, I lock the dimension by clicking on the little lock icon. This will prevent the edit to the 0.875 dimension from altering this edit.

I click enter to accept the dimensional change. Notice that the new value is in red, indicating a locked state.

Live sections are subject to the same live rules as 3D editing. Therefore, since this part is symmetrical about a base plane, I only have to edit the one side and the other side automatically updates.

Next I modify the 0.875 dimension to 0.375, again making sure that the directional (red) arrow is pointing to the side that will move.

Since this is the last dimension I will edit here, I choose not to lock it.

Once again the symmetric live rule updates the other side for me.

Next I have to place some cutouts into the roller. Although I will do this on the 3D model, I can use the live section to help me accurately place the initial cutout sketch, as shown below:

I then show the Design Body and hide the Live Section

Using the Revolve command, I set the selection type to Face and select the sketch region, created by my sketch and the edge of the cylinder.

I RMB click to accept this selection. Notice the Axis icon activates and you will be prompted to select the axis of revolution.

I move the cursor over the large cylinder and the axis of the cylinder highlights for selection. I select this axis.

I then ensure that this will be a revolved cutout by selecting the remove option.

Next, I select a full 360 degree revolution.

And I have created my first groove, accurately positioned and dimensioned.

To complete the model I use the Rectangular Pattern command. I first select the newly created Revolved Cutout from the PathFinder.

Then I select the Rectangular Pattern command.

I select the Right(zy) reference plane to place the preview of the pattern.

Note: The synchronous pattern command automatically generates a preview of a default pattern and provides on screen dynamic input boxes for you to enter your desired parameters.

In this scenario, I entered the following values.

  • - X Count: 14
  • - Y Count: 1
  • - X distance of 14”
  • - Because the Y Count is 1, I don’t have to enter a Y distance.

 

I RMB click to accept the pattern and model is complete.

Notice that if I hide the PMI dimensions and turn on the Live Sections, my live section has updated to include the grooves.

Notice that in this scenario we could have modified this part using just the 3D model and steering wheel to adjust the ends. We could have also just used 3D dimensions directly on the model. However, using the live section provides some users with a comfort level and easier visualization, similar to working in the ordered environment.

I think it’s also worth mentioning that if this model had been designed in another CAD package, the exact same steps would be used to make the exact same edits. With synchronous technology, the user can take any CAD model and work with it as if it was modeled in Solid Edge.

For additional information, please see the topic Live Section command in Solid Edge Help. A training activity for this command is located in the self paced training section. Follow this link http://www.solidedge.com/spt/en/ST4/spse01520/book.html, and then click on the Working with Live Sections chapter.

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