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Tips - 2


Question: How do you change a parameter type (i.e. string to real number)?

Answer 1: Using the Model Tree: Create a column in your model tree under model parameters the same name as the parameter you want to change (this is a good way to enter values too). It should display thevalue of the parameter. Click on it and use 'backspace' to clear the field. Don't hit enter, just arrow (or pick) to a different field. If you pick on the (now empty) field of the parameter you just erased, it should give you a pop up to choose "string, integer, etc." and you're off! I've seen it take more than once to get the field clear, so if it doesn't take the first time, give it another shot.

Answer 2: Using Pro/PROGRAM: If you will open the pro/program of the part file and in the input section type in the parameter name and type this will change the parameter type. For instance if you have a parameter called "TEST" that used to be an integer and you want to change it to a string variable the pro/program will look like the following: INPUT TEST STRING END INPUT To test if the change was made use the info under the parameter selection to look at what is assigned.



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Did you know you can add parameters to the model tree? If you call up an assembly and add the parameter rev to the model tree then you can add that parameter to every part from the model tree without calling up the parts individually.



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Question:Can I specify the color of the part as item in a family table?

Answer: Yes, you can: you first must set a parameter named color,if you'd like, with a value "black" for instance. Then "add item" to the family table (Fam table/add item) and select "parameter/color" from the menu. Of course, your initial value (black)will be attributed to your generic model. You can add an instance that on the "Color" column would have any another value(natural,etc). You can see your model parameters in the tree by adding the column for the model parameters.



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Question: Can I show the dimension symbol rather than a value for shown dimensions in a drawing?

Answer: Try this. In a drawing, modify a dimension. Under the DIM TEXT tab, change the @d to @s and change the name of the dimension in the appropriate box. This will only change the dim to a small string and cannot be used for multi-line text.

Thanks to weeble.net for helping us modify the site and blogmatters for some tweaks.


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Question: How do I control line weight on my plots?

Answer: Try adding these lines to your config.pro file or loading it as its own pen weight file. Change the numbers as required.

plot_linestyle_scale 1
pen1_line_weight 1
pen2_line_weight 1
pen3_line_weight 1
pen4_line_weight 1
pen5_line_weight 1
pen6_line_weight 1
pen7_line_weight 1
pen8_line_weight 1



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Question: How can I break a large table into multiple smaller tables?

Answer: You can do both through Pagination, found under Table. #Table;#Pagination;#Set Extent;#Add Segment. When you add a segment, you can set the extent of that segment as well and go into 3 or more columns. If you go to the next page before you add a segment, the new segment will be on the next page.



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Question: How can I tell which version a Pro/E model was made in?

Answer: Open up the .prt file in a text editor and look at the first line. It yields the necessary information. for example. #UGC:2 ASSEMBLY 1068 440 0 1 1 15 2100 2000050 0000b335 \ #- VERS 0 0 \ #- HOST in this listing, the 2100 signifies v21 or 2000i and 2000050 is the build.



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Question: Does any one know how to use a silhouette edge of a parallel blend? I'm tring to grab it as a reference in another sketch, but I can only select the surface of the blend, not the edge.

Answer: What I do is this. #Geom Tools #Xsec Ref Ent, and pick the surface that the silhouette edge belongs to as the 'reference surface' that intersects the sketching plane. Then you can sketch an entity that snaps to this reference entity. It will produce the same effect that you're looking for. There may another way to pull this off, but this is what I've had to resort to. I do believe that the #Xsec Ref Ent functionality was added for this very purpose.



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Question: Is it possible to "purge" unused symbols from a drawing?

Answer: Under the Detail menu, choose Create ; Symbol ; Definition ; Delete.



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Question: How do I add default datum planes to an existing model?

Answer: Use this procedure to add default datum planes to an existing assembly as the first three features.

1. Add a placeholder CSYS feature as feature #2.
Pick #Feature; #Create; #Datum; #Coord Sys; #Default; #Done; #Done/Return; #Feature; #Reorder (reorder the new CSYS to be feature #2) #Done/Return

2. Suppress the first feature and all its children. Pick #Info; #Regen Info; #Beginning; #Fix Model; #Quick Fix; #Suppress; #Suppress All; #Quit; #Yes

3. Use 'Fix Model' to create the planes before the first feature. Pick #Info; #Regen Info; #Beginning; #Fix Model; #Fix Model; #Feature; #Create; #Datum; #Plane; #Default; #Done/Return; #Done/Return; #Quit

4. Resume all the suppressed features. Pick #Feature; #Resume; #All; #Done; #Done/Return

5. Delete the placeholder feature. Pick #Feature; #Delete, pick the placeholder CSYS feature, #Done Sel; #Done; #Done/Return

6. Check the model tree. Be sure 'Tree, Show, Features' is checked on. The new planes are now the first three features of the assembly.



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Question: Can I specify what folder Pro/E defaults to when opening new models?

Answer: Use the config.pro option: "file_open_default_folder"



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Question: How do I reroute or redefine a radial placed hole? Pro/E doesn't seem to give me the correct references.

Answer:
1) Redefine hole.
2) Change to Linear Type... Don't select any references. Just hit Done Sel.
3) Change back to radial and reselect the references.



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Question: Can a dimension be placed in a note while remaining in the view where it was shown? When using the "&d" in a note, it disappears from the view (unless it is an angular dimension). I would like to have the dimension update in the note where it is referenced and in the view.

Answer: Create TWO notes with the dimension "&d" then delete the first one.



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Question: Can I write a relation to fill in the empty blanks in a repeat region of a table?

Answer: There is a simple way to do it, although there is important one key: Make sure that the user-defined repeat region parameter that you create at the table is from Pro/REPORT, NOT a model parameter. That repeat region parameter must have nothing to do with the part. Then via relations, you assign values to the repeat region parameter based on (in my case) the model name (asm.mbr.name). I added a parameter to the repeat region called "table_title" (Relations > Add Param > String) and did not assign it any initial value. Then I made the first cell of that column point to the "table_title" parameter (Enter Text > Report Sym > rpt. > rel. > User Defined > table_title). Next, I added relations to the table as follows:

if asm_mbr_name == "T1004011"
table_title = "RETAINING RING, TURARC INT, .50 10 N5000-50C"
else
if asm_mbr_name == "B038950"
table_title = "DOG, .495 DIA X .500 LG, 6.75 ARC"
else
table_title = asm_mbr_title
endif
endif

The parts that did not have a title parameter are listed first, then assigned a description to the "table_title" parameter (remember, it's only a Pro/REPORT parameter). Otherwise, the remaining parts' model paramter "TITLE'" is assigned to the "table_title" parameter for the repeat region. Works like a charm!



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Question: How do you create a Parametric Note which will show the Volume of a part?

Answer: It is very simple. Create a parameter called VOLUME. Create a relationship VOLUME = MP_VOLUME(""). You must use model analysis to calculate the volume. This is not done automatically. Sometimes I also have to go into the relations menu and sort the relations to get the VOLUME parameter to update.


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Question: Is it possible to show tolerances on dimensions that you overide with the @O or @S command?

Answer:
To create superscripted text: type [@+text@#]
To create subscripted text: type [@-text@#]
'Text' is the note text that is superscripted or subscripted.
The '@#' is to end the sub/super script.

So your dimension line would read {{0:@O}1.000 @++.005@#@--.002@#}.

This would mean your dimension and tolerance is non-parametric.



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Question: How can I control the number of decimal places that a value gives in a note?

Answer: Modify the text to read '&<parameter name>[.#]', where [.#] specifies the number of digits to use to the right of the decimal.



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Question: Can I make a "regular" part from a skeleton part?

Answer: If your skeleton has no external references, you can make a new part from it by starting a new part and using "copy from ..."



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Tip!

Create round features on your model as late in the design as possible. Do not dimension other features to the edges or tangent edges of round features. This may create unwanted dependencies on the round feature by other features. This may make feature manipulation more difficult later in the design process.



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Tip!

When selecting curcular edges for chamfers, Pro/E only highlights one half of the edge. Pro/E places the chamfer on the entire circular edge, so you don't have to select the other half of the edge.



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Pro/ENGINEER is:

Feature-based -- Pro/E builds the model one feature at a time. A feature is the smallest building block in a model. Building your model with simple features makes your part more flexible.

Associative -- Changing the design at any level will automatically change the design at all levels. For instance, you can change a dimension in a drawing, and the resulting change will be reflected in the part and assemblies instantly.

Parametric -- Features of the model are interrelated. Modifications of a single feature propagates changes in other features as well, preserving your design intent. A relationship between features develops when one feature references another and is known as a parent/child relationship.



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Reminder!

When you orient a datum plane (top, bottom, left, right, front, back) the yellow side of the datum plane faces that side of the computer screen.



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Tip!

External references of a sketch (section) are identified by a brown dashed line in sketcher mode.



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Tip!

Dimensioning in a 3D view helps avoid unwanted parent/child relationships. This allows you to see clearly which reference you are picking, and helps you pick surfaces rather than edges.



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Tip!

Open or closed section? When in doubt, use a closed section. It is easier to regenerate and is less prone to failure.



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Tip!

In Intent Manager, use the right mouse button to disable and lock highlighted constraints. Right-clicking disables the constraint, +right clicking locks the constraint. To toggle between different constraints, use the key.



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Remember!

A sweep can fail if a sweep trajectory radius is too small relative to the section, and the section intersects itself while sweeping along the trajectory.



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Tip!

Add relations as soon as you know you need them. Document the relations by using /* before a comment line. Pro/E ignores anything after the /* for that line. This allows you to write notes to yourself and others.



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Tip!

Do not use a sketched centerline to create a rotational dimension. Centerlines have no direction associated with it. Use a make datum instead.



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Question: How can I tell what directory the part I'm working with is from?

Answer: Set your config.pro setting, "display_full_object_path" to "yes".

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