Posts Tagged ‘Solid Edge Synchronous Technology ST STEP IGS’

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Integrated Modeling in Solid Edge

Monday, November 19th, 2012handbook

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete
the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses. For more information visit our website at http://www.designfusion.ca//synchronous_tech_course.php. New 2013 courses will be added to our schedule soon.

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Understanding the Steering Wheel

Tuesday, October 16th, 2012

Many traditional users have expressed some concern over the use of the steering wheel in synchronous technology. They find it complicated or cumbersome to use. However, once they receive proper training they all agree that it is a powerful and useful tool that is really quite easy to use.

The basics of the steering wheel allow the user to move faces in a linear, rotational or freeform move, similar to the Drag Component command in the assembly environment. The primary and secondary axes allow you to perform linear moves. The torus allows you to perform rotational moves. The tool plane allows you to perform freeform planer moves. With a little knowledge you can quickly and easily move or rotate faces or face sets as required. The notes below are what our trainers hand out, in our courses, and illustrate a few simple ways to control and position the steering wheel.

The steering wheel components

Positioning the steering wheel
When you want to rotate the steering wheel 90° on an axis that is NOT defined by the primary axis of the steering wheel, hold down the Shift key and Click the small blue plane inside of the steering wheel.
  • Shift + Click the Tool Plane will flip the steering wheel 90° about the axis NOT aligned with the primary access.

  • You can also Ctrl + Click the primary bearing knob at the end of the primary axis and key-in an angle.

When you want to rotate the steering wheel 90° on an axis that is defined by the primary axis of the steering wheel, pick the bearing knob on the secondary axis of the steering wheel and drag to rotate.
  • The steering wheel will snap to 90°.

  • You may also Shift + Click the bearing knob at the end of the secondary axis and key-in an angle.

Once you get the steering wheel in the desired orientation, Shift + Click the origin of the steering wheel to relocate it.
  • No need to continue to hold down the Shift key after clicking
  • It will not flip orientation.
  • Secondary axis will not realign to an edge

Changing the Primary Axis Vector

You can change the direction of the primary axis by doing one of the following:

  • Click on any of the 4 positional knobs.

  • Click on the primary bearing, hold the LMB down and align with any keypoint.

For more information on the steering will you can check out the online training section on ‘Moving and rotating faces’ at http://www.solidedge.com/spt/en/ST5/spse01520/book.html or attend one of our synchronous training courses. If you are a regular follower of this blog, you may recall the article on training, where it mentioned that one hour of instructor lead training is equivalent to 16 hours of trying to teach yourself. For more training information please visit our training site at http://www.designfusion.ca//training_schedule.php.
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Using the mouse to manipulate the model view in Solid Edge

Thursday, June 21st, 2012

The middle mouse button, or scroll wheel, provides improved model rotation in ST4. You can now select a vertex, edge, or face as the model rotation center. To do this, simply following the steps below:

First you must let the system know that you want to enter the rotation mode. This is achieved by a single click to the middle mouse button (MMB), on an empty space. You will notice the cursor changes appearance. Before you click the MMB your cursor looks like this:

                    

After you click the MMB you cursor will look like this:

  

Notice that the little blue face, indicating selection mode, has disappeared.

You now have three options available to you: 

 

1. Rotate using a position on a face.

  •  - You can now move the cursor over the face shown below. Notice the dark pink dot, indicating that you are in the rotate mode.

 

  • - If you now hold the MMB down, the part will rotate about the dark pink dot. In other words, the dark pink dot becomes your center of rotation.

 

2. Rotate using a position on an edge.

  • - You can move the cursor over any edge. Notice the entire edge highlights.

 

  • - Holding the MMB down allows you to rotate about the edge. In other words, the edge becomes the axis of rotation.

 

3. Rotate using a position on a vertex.

  • - You can move the cursor over any circular edge. Notice the entire edge highlights.

 

  • - Holding the MMB down to rotate allows you to rotate about the vertex of the circular edge. In other words, the vertex of the circular edge becomes the axis of rotation.

 

Note:  Once you have completed the rotation, you are returned to selection mode. You will have to single click to the middle mouse button (MMB), on an empty space, if you wish to perform another controlled rotation.

 

Other handy mouse controls in Solid Edge

 - Pan the view. Press the Shift key while you drag the MMB to pan the view.

 

- Zoom. Scroll the mouse wheel to zoom in and out.

 

Note: The setting for this scroll behavior is found in Solid Edge options_Helpers page. Enable Value Changes Using the Mouse Wheel. If this option is on, the mouse wheel changes the value in a value edit field. Use Ctrl+mouse wheel to zoom in or out.

- Zoom Area. Press the Alt key while you drag the MMB to zoom into an area.

- Double–click the MMB: Fits the view.

 

Creating insert notches in sheet metal

Thursday, May 17th, 2012handbook

Recently I was asked if Solid Edge had a special command for making insert notches in sheet metal. These notches are used to insert tabs or pins in various assemblies. The image below shows a few examples of the type of notches I refer too.

 

To create these notches and others like them, I always use the Bead command in the Solid Edge sheet metal environment. Although designed to create beads, it also creates open ended beads, which are notches. To do this you start with a sketch which represents the length of the bead. For example, I may need a 6.35mm (1/4 “) wide notch, so I create a 6.35mm sketch line.

Using the bead command options, I select the overall shape of the notch. For example, I may need a U-shaped notch 6.35mm high and 10mm wide.

Notice that I set a lanced end condition. I could also use a punched end condition which allows me to extend the cutout portion of the notch.

If this is a feature that I will use often, I can save the settings for easy recall in the future.

Once I say OK to the options dialog, I simply select the direction that I wish to apply the notch.

The resulting bead feature can be edited by adjusting the options or editing the sketch. It can also be added to a feature library.

So my answer to the original question:  “Does Solid Edge have a special command for making notches in sheet metal?” is yes. It’s called the Bead Command.

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Is Training Worth It? – Calculate your Return On Investment

Tuesday, March 27th, 2012

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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