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A “Quicksheet” is a template of drawing views that are not linked to a model. You can then drag a model from the Library tab or from Windows Explorer onto the template, and the views populate with the model. If you have standard views on a particular size of drawing, for example, you can have the Draft preconfigured to populate itself based on the model you place on the sheet.
You will to need to set up a Draft sheet (but do not use production drawing as the drafting information will be removed upon save) with your views and other items such as Parts Lists.
1. Go to the SE Application button
2. From the Application menu, choose the “Create Quicksheet Template” command.
3. Save the file to a location and give it a name that easily identifies it. It is best to place this on a network area other users can get to if it is useful to share the Quicksheet. It is also best to locate it in a similar area to where the company templates for SE reside.
* Almost all view properties, including general properties, text and color properties, and annotation properties, are maintained. However, some display properties, such as selected parts display, Show Fill Style, and Hidden Edge Style, are not maintained.
Now a Quicksheet template has been created, but how do we use it?
1. Open your Quicksheet template (either through Windows Explorer or if you set up your User Templates and placed the Quicksheets in that location hit New>Quicksheet> and select your Quicksheet).
2. Drag and drop your desired Part or Assy onto the sheet from Windows Explorer or through the Library tab in Solid Edge.
3. Solid Edge will place the geometry and will be ready for the next steps.
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
• Locate, select and edit of ordered features
• Edit synchronous procedural features
• Delete synchronous face-sets and ordered features
• Move face-sets (sync feature) in synchronous parts
Over the years I have noticed some gems in Solid Edge that I would like to share. Quick Query I feel is a small but powerful little nugget. I will list the steps below to perform a quick query in assembly and also try to state some benefits to this. Trust me it takes longer to explain than to do.
Firstly it is important to note that parts and assemblies have properties embedded in them. These fields should be used for a multitude of reasons from parts lists to searches. It would be important for all to understand this before moving on. Obviously these fields must have information in them in order for Solid Edge to report back anything.
Below I have an example part that exists in the example assembly I will use.
To check the properties
We can check what has been entered by going to the part properties. Select the Solid Edge application button and go to Properties>File Properties.
You can also look at the property manager, which will be discussed at a later date, or perhaps through automation if you have a custom program to assist in entering this data.
As you can see below we have an entry of “hardware” in the “Category” field. This is what we will perform a quick query on later.
We now return to the assembly.
Click on the “Select Tools” tab.
Perform a quick query
RMB in the blank area just below the words in the title bar that say “Select Tools” and the following menu appears. Note that these options correspond to those fields we had seen in the part properties. You can set up a search to find these items based on these same categories.
You can see the many choices presented to you for searching. Any one of them can be used. For this example we will search the “Category” field.
Let’s set up a Quick Query to find and part in the assembly with the word “hardware” in the “Category” field. We RMB in the blank area, and select “Category”. This sets the Quick Query option to search the “Category” field in all parts and select and highlight all that contain the word “hardware”.
Once the text has been entered, press the enter key and you should have all the parts highlighted and selected like below:
Note that the highlighted parts are any that contain the word “hardware” in the “Category” field. This search went into sub assemblies and patterns to select items. It would also select different items as long as the field had the word hardware in it. You could do a “Show Only” or other options for the selected set of parts.
There are many applications for this tool (another time we will discuss a full Query). Quick Query is very useful. It can select a set of items so you can do things like double check quantities or locations. Also, because it shows only items matching the query, it can help determine if an item might also be missing properties. This is good to know especially if those fields are required for a parts list in draft for example.
The most common use of Part Families is to define a standard library part that has many variations.
1. Create a hexbolt
2. Rename the expression that you want to keep
a-Width = the radius of the cap
b-Length = length of screw
3. Define the columns for the Family Table.
Choose Tools→Part Families from the main menu bar.
Make sure the Importable Part Family Template option is cleared.
Click OK on the Warning dialog box.
Select the width expression from the top window of the Part Families dialog box.
Click the Add Column button.
Select the length expression from the top window of the Part Families dialog box.
Click the Add Column button.
Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.
Change the option menu at the top of the dialog box from Expressions to Features.
Double-click chamfer from the top list of the Part Families dialog box.
The order in which you select the attributes determines the order of columns in the spreadsheet.
In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.
4.Create the family table.
5.Verify a family member
Select a cell in row 3.
From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.
The NX session becomes active and the family member is displayed in the graphics window.
Click Resume in the Part Families dialog box.
The Part Families dialog box may be obscured, if so, click anywhere in the NX window.
6.Save the Part Family and the template part.
From the spreadsheet menu bar, choose PartFamily→Save Family.
The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.
In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.
Since we do not use this part anywhere else we are not going to do that.
7.Close all parts.
Currently, the NX Thread command can be used to create a fully modeled straight thread. When
this command is run and the Detailed Thread type is selected a fully modeled thread will be
created. NX provides Modeling tools which allow users to create fully modeled tapered threads.
The Variational Sweep is one of these tools.
1. Create a Datum CSYS on the centerline of the thread at the start location of the tapered
2. Create the following expressions in the Expression editor.
ANGLE will be the included angle of the thread profile. This is typically 60 degrees.
L will be the length of the thread.
P is the thread Pitch which is the distance from thread to thread.
START_DIA is the diameter at the start end of the thread.
TAPER is the taper of the thread.
END_R will be the calculated value L*TAN(TAPER)+STRT_R.
STRT_R will be calculated as START_DIA/2.
All expressions should be created as Length type expressions except for the ANGLE
and TAPER variables. These two need to be set to the Angle expression type. If these
variables are not created as Angle type expressions they will not be selectable when
creating the feature.
3. Start the process by creating a Helix curve.
The Number of Turns will be calculated by dividing the Length by the Pitch or L/P using
the defined expressions. The Pitch variable will be specified using the expression P.
4. To create the tapered helix the Radius Method Use Law will be used. When selected
the Law Function window will be displayed. At this point select the Linear type.
5. Specify the Start and End radius values by supplying these expression variables.
Note that the tolerance of the helix can greatly influence the accuracy of the thread.
Initially the helix will be created to the model tolerance in effect when created. This can
be found at Preferences => Modeling => Distance Tolerance.
If the accuracy needs to be improved after the helix is created a higher tolerance can be
specified by editing the helix and changing the tolerance value.
6. After the helix is created select Insert => Sweep => Variational Sweep. Select the helix
curve as the path. For Plane Orientation pick the Through Axis option and select the
centerline of the helix for the vector. For the Sketch Orientation select the same axis.
7. When OK is pressed a Sketch will be created. At this point create the profile of the
thread. Constrain all geometry to the point that was created on the helix curve when the
Variational Sweep operation was started. This is an important step.
It is significant that the width of the thread be smaller than the Pitch (P-.01). If this width
value is too large then the model will intersect itself as it sweeps along the helix guide
curve. This would cause an invalid solid to be created.
8. When the sweep is complete a hollow thread profile will be created as seen below.
9. The thread would be completed by Uniting it to the model of the base of the thread.
This same procedure can be used to create a multi-lead thread. When creating the
Variable Sweep Sketch of the thread profile create two threads at half the Pitch in width.
See the sketch below along with the picture of the resultant multi-lead thread. The colors
of the different leads have been altered for emphasis.
Using tools provided in NX, users can quickly and easily model complex features.
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|
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.
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.
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.
With NX8, the pattern command got a fresh new look and more command features associated with it.
One of the new features is the simplified boundary fill; this feature will fill the specified face with three different pattern layouts;
This can easily be done in a single pattern, so no more having to position the origin of the feature, just select the feature, select the boundary face and voila!