Creo Parametric Tips

This is a document so please edit it and add, correct, &/or clarify how you see fit.  Then we can all use this as a point of reference when dealing with Repeat Regions/BOM programming.  If you don't want to edit it but still want to contribute, then just leave a comment.  Thanks!   List of System Parameters and Model Parameters used in model/drawing (Document - CS133915): https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS133915&art_lang=en&posno=10&q=repeat%20region%20symbols&sourc…   List of Operators and Functions: Type Name syntax Explanation eg: Input   Eg: output Assignment Operator = MyVar="string" Defines, or assigns, a variable as a # or string       MyVar="H123" MyVar=10     = = No Output but defines the variable MyVar to be: H123 10 String Operators/Functions   Comparison Operators ==     == A==B     #A==#B Compares strings as equal.     Compares #s as equal "456"=="123" "456"=="456"   7==1 7==7 = =   = = NO YES   NO YES String Operators/Functions     Comparison Operators !=, <>, ~= A!=B A<>B A~=B   #A!=#B #A<>#B #A~=#B   Compares strings as unequal. (checks to see if not equal or not)     Compares #s as unequal. (checks to see if not equal or not)   "456"<>"123" "456"<>"456"     7!=1 7<>1 7~=1 7!=7 7<>7 7~=7 = =     = = = = = = YES NO     YES YES YES NO NO NO String Operators/Functions Arithmetic Operators +   + A+B   #A+#B For Strings: Concatenate strings. For Numbers: Add #s (Addition, Plus) "456"+"123"   7+7 =   = 456123 (returns a string e.g. "456123"*1="ERROR") 14 Arithmetic Operators - #A-#B Subtract #s (Subtraction, Take away, Minus) 3-2 = 1 Arithmetic Operators / #A/#B Divide #s (Division) 6/2 = 3 Arithmetic Operators * #A*#B Multiply #s (Multiplication) 6*2 = 12 Arithmetic Operators ^ #A^#B A to the Power of B (Exponent, Powers, Raised to) 2^3 = 8 Arithmetic Operators () (#A-#B)*#C Parentheses for grouping, Priority, and order of operations (3-2)*4 4*(3-2) = = 4 4 Comparison Operators ==   <See String Operators above>       Comparison Operators > #A>#B Greater than       Comparison Operators >= #A>#B Greater than or equal to       Comparison Operators !=, <>,~=   <See String Operators above>       Comparison Operators < #A<#B Less than       Comparison Operators <= #A<#B Less than or equal to       Comparison Operators | #A | #B | #C OR       Comparison Operators & #A & #B & #C AND       Comparison Operators ~,! #A == !B     #A!=B #A~=B NOT (i.e. Reverse a statement, Opposite) (                         Tilde ~ doesn't work for NOT next to a #.  Only next to operator = 7 == 7 7 == !7 7 == !4 7> 4 7>!4       7 != 7 7>=3 7!>=3 7~=7 7~=4   7 == ~7 7 == ~4 "ABC" == !"ABC" = = = = =       = = = = =   = = = YES NO NO YES YES (I guess even mathematically this is strange)   NO YES NO NO YES   ERROR ERROR ERROR Mathematical Functions abs abs(#) Returns the absolute value of a number abs(-2) = 2 Mathematical Functions acos acos(#º) Returns the arccosine of a number ACOS(0.125) = 1.445468496 Mathematical Functions asin asin(#º) Returns the arcsine of a number ASIN(0.125) = 0.125327831 Mathematical Functions atan atan(#º) Returns the arctangent of a number ATAN(0.125) = 0.124354995 Mathematical Functions atan2 atan2(#º) Returns the arctangent (inverse tangent), of the specified x- and y-coordinates ATAN2(2,3) = 0.982793723 Mathematical Functions bound bound(#x,#lo,#hi) Forces #x to be within the range of #lo to #hi. If x ≤ lo,        then output = lo. If lo ≤ x ≥ hi, then output = x If x ≥ hi,        then output = hi   (kind of the opposite as DEAD(), but not exactly)     bound(0,5,15) bound(7.25,5,15) bound(100.2,5,15)     = = =     5.0 7.25 15.0   cable_len       =   Mathematical Functions ceil ceil(#) Round # up ceil(3.25) = 4.0000   comparegraphs       =   Mathematical Functions cos cos(#º) Returns the Cosine of a # cos(2) = -0.416146837 Mathematical Functions cosh cosh(#º) Returns the hyperbolic Cosine of a # cosh(2) = 3.762195691   dbl_in_tol  dbl_in_tol (#x, #y, #r) Checks to see if x and y are within the tolerance of ± r #x, #y, #r are all real numbers Returns TRUE if abs(x-y) ≤ r Returns FALSE if abs(x-y) > r dbl_in_tol (2, 1, 1) dbl_in_tol (2,1,0.5) dbl_in_tol (10,20,9) dbl_in_tol (10,20,10) dbl_in_tol (10,20,11) = = = = = YES NO NO YES YES Mathematical Functions dead dead(#x,#lo,#hi) "Defines a range of values for x, for which the result of the function is 0." If x < lo,        then output = x–lo If lo ≤ x ≥ hi, then output = 0 If x > hi,         then output = x–hi   (kind of the opposite as BOUND(), but not exactly)     bound(0,5,15) bound(7.25,5,15) bound(100.2,5,15)     = = =     -5.0 (0-5) 0 85.2 (100.2-15) Cabling, Case Study Functions eang  eang(e_ID1, e_ID2)  Angle in radians between two entities, e_ID1 and e_ID2, of a case study   =   Cabling, Case Study Functions ecoordx  ecoordx(e_ID1)  x coordinate of the e_ID1 entity of a case study   =   Cabling, Case Study Functions ecoordy  ecoordy(e_ID1)  y coordinate of the e_ID1 entity of a case study   =   Cabling, Case Study Functions edistk  edistk(e_ID1, e_ID2) Distance between two entities, e_ID1 and e_ID2   =   Cabling, Case Study Functions elen  elen(e_ID1)   Length of the e_ID1 entity of a case study   =   Graph Evaluation Function evalgraph  evalgraph("graph_name", x) Graph evaluation function enables you to use graph features to drive dimensions through relations. The dimensions can be section, part, or assembly dimensions. graph_name—the name of a graph. x—the value along the x-axis of the graph for which the y value is returned.   =   Strings as Arguements exists  exists("x") Test if a parameter, variable, or dimension exists or not   x is a string EXISTS("ASM_MBR_NAME") EXISTS("ASM_MBR_NAME_") EXISTS("test03") = = = YES NO YES (note test03 is a defined variable in my relations) Mathematical Functions exp exp(#) e3 Returns e raised to the power of a number, where e = Euler's number = 2.718…  exp(3)=e3 =  20.085537 String Operators/Functions extract extract(#1,#2,#3) Extracts pieces of strings. #1=string analyzing #2=starting position #3=length (how many char to extract)   e.g. looking at the entire string (4324870B) Starting with the first character (4) Extract 7 characters (4324870) extract("4324870B",1,7)   Extract("4324870B",8,1) =   = 4324870   B Logical Functions False* false() false False function Returns "No" (For some reason doesn't return "False"!) False() False = = NO FALSE Mathematical Functions floor floor(#) Round # down Floor(3.25) = 3.0000 Mathematical Functions if IF(c,x,y) Similar to IF() function in Excel: c= condition statement x = what to do if true y= what to do if false (PTC documentation calls this a switching function but to me is too  basic to earn this title) IF(10==9,2,10) = 10.0 Conditional Statements if, Else, Endif IF <condition>    <what to do if condition is met>   ELSE <what to do if condition is not met> (optional)   ENDIF If--Starts the if statement Else--says what to do if statement is not bet (and is optional) Endif--(closes the if statement)   Can have IF without ELSE Can't have IF with more than one ELSE (E.g. IF ELSE ELSE ENDIF Can't have IF without ENDIF Can have nested IF statements.  Eg. IF ELSE IF ELSE IF ENDIF ENDIF ENDIF asm_mbr_name = 4564870B IF string_length(asm_mbr_name) > 7    Test01 = extract(asm_mbr_name,1,8) ELSE    Test01 = extract(asm_mbr_name,1,7) ENDIF = 4564870B String Operators/Functions itos itos(#) Integer to String-- Reads in an integer and returns a string.  If the input number is a # that is not an integer, itos rounds up, than converts to a string. itos(6) itos(6.7) = = 6 7 Mathematical Functions ln ln(#) Returns the natural log (base e) of a # ln(2) = 0.693147181 Mathematical Functions log log(#) Returns the base 10 logarithm of a # log(2) = 0.301029996   lookup_inst lookup_inst ("generic_name", match_mode, "param_name_1", match_value_1, "param_name_2", match_value_2,...) Used in ProPROGRAM Used to automatically replace the given Family Table instance with another FT instance: •generic name—Name of the generic model with a prt or asm extension •match_mode—One of the following values: –1 (find closest instance with param values less than or equal to supplied values) 0 (find instance with param values that match supplied values exactly) 1 (find closest instance with param values greater than or equal to supplied values) •param_name_1—Family table parameter name •match_value_1—Value to match against INPUT END INPUT RELATIONS INST_NAME = LOOKUP_INST ("PEG.PRT", 0, "D2", D6:0, "D1", D5:0 + 1) END RELATIONS ADD PART BLOCK INTERNAL COMPONENT ID 1 END ADD ADD PART (INST_NAME) INTERNAL COMPONENT ID 2 PARENTS = 1 (#1) END ADD MASSPROP END MASSPROP Example: Replacing Family Table-Driven Components --> "In this way, the instance of peg.prt being assembled to blockpeg.asm is controlled, based on the dimensions of the hole in block.prt."     massprop_param       =     material_param       =   Mathematical Functions max max(#) Compares 2 #s and returns the larger one max(6.2,4) = 6.2 Mathematical Functions min min(#) Compares 2 #s and returns the smaller one min(6.2,4) = 4 Mathematical Functions mod  mod(#n,#d) Modulus function.  Also known as Remainder function because gives just the remainder. e.g. n/d (numerator/denominator): 10/2=5 Remainder=0 (10/2+0/2) 10/3=3 Remainder=1 (9/3+1/3) 10/4=2 Remainder=2 (8/4+2/4)   In Programming Modulus can be useful to do many things. e.g. Determine if Number is Odd/Even [if mod(n,2)=0 then n is even] Clock arithmetic [mod(9+5,12)=2pm] Truncating decimal values Wrapping values into a certain range [given mod(n,360) to determine what quadrant a particular angle falls in for the unit circle) if Remainder       0-90, then Quad.1 if Remainder   90-180, then Quad.2 if Remainder 180-270, then Quad.3 If Remainder 270-360, then Quad.4]       Mod(10,2) Mod(10,3) Mod(10,4)           Mod(9+5) Mod(9+8,12)     Mod(400,360)   Mod(2300,360)       = = =           = =     =   =       0 1 2           2 (e.g. 9am+5hrs =2pm) 5 (e.g. 9am+8hrs = 5pm)     40 (40º is in quadrant 1)   140 (140º is in quadrant 2)   mp_assigned_mass       =     mp_cg_x       =     mp_cg_y       =     mp_cg_z       =     mp_mass       =     mp_surf_area       =     mp_volume       =   Mathematical Functions near near(#y,#y,#delta) determines if the numbers x and y are within delta of each other near(5,8,3) near(5,8,1) = = 1.0 (i.e. when true) 0.0 (i.e. when false) Logical Functions No* no() no No Function Returns "No" No() No = = NO FALSE Mathematical Functions pi pi() Returns the number for PI PI() = 3.141592654 Mathematical Functions pow pow(#x,#y) x^y Raising x to the Power of y #1=Base value #2=Exponent Pow(1,2) Pow(2,2) Pow(2,4) = = = 1.0 (i.e. 1^2) 4.0 (i.e. 2^2) 16.0 (i.e. 2^4) Strings as Arguements rel_model_name rel_model_name   or   rel_model_name()     Passing Strings as Arguments in Relations rel_model_name   rel_model_name()   =   501234 (when done on 501234.drw table repeat region relations) Strings as Arguements rel_model_type   rel_model_type   or   rel_model_type() Returns the current model type.  If you are working in Assembly mode, rel_model_type() is equal to assembly.   (note you can use with or without parenthesis) Passing Strings as Arguments in Relations rel_model_type   rel_model_type()     = DRAWING (when used in table repeat region relations) String Operators/Functions search search(string, substring) Searches for substrings. The resulting value is the position of the substring in the string (0 if not found). You can specify substrings with single or double quotes. search(asm_mbr_name,"501234") = 2 (Given asm_mbr_name is 05012340.prt) Mathematical Functions sign  sign(x,y)  Sign Transfer of y to x If y<0, the result is –abs(x) if y>=0, the result is abs(x). sign(-2,3) sign(2,3) sign(2,-3) sign(-2,-3) = = = = 2.0 2.0 -2.0 -2.0 Mathematical Functions sin sin(#º) Returns the sine of a number sin(2) = 0.909297427 Mathematical Functions sinh sinh(#º) Returns the hyperbolic sine of a number sinh(2) = 3.626860408   smt_def_ben_rad       =     smt_thickness       =   Mathematical Functions sqrt sqrt(#) Take the square root of a number sqrt(4) = 2 String Operators/Functions string_ends string_ends (string1, string2) Check to see if string1 ends with string2 Case Sensitive ("H" <NOT => "h") string_ends("h456","56") string_ends("h456H","56h") string_ends("h456H","56H") = = = YES NO YES Strings as Arguements string_length string_length(string)   string_length(<param>) Returns the number of characters in a string or parameter. string_length("als23fj") string_length(asm_mbr_name) = = 7.0 6.0 (when done on 501234.prt table repeat region relations) String Operators/Functions string_match string_match(string1, string2) Check to see if 2 strings are exactly the same or not Case insensitive ("H"="h") string_match("456","456") string_match("456","4560") string_match("h456","H456") = = = YES NO YES String Operators/Functions string_starts string_starts(string1, string2) Check to see if string1 starts with string2 Case Sensitive ("H" <NOT => "h") string_starts("h456","h4") string_starts("h456","H4") string_starts("h456","asd4") = = = YES NO NO Mathematical Functions tan tan(#º) Returns the tangent of a number tan(2) = -2.185039863 Mathematical Functions tanh tanh(#º) Returns the hyperbolic tangent of a number tanh(2) = 0.96402758   trajpar   "Trajectory Parameter" Returns a system of numbers that varies from 0 to 1 across the length of a given path http://en.wikipedia.org/wiki/Trajpar sin(trajpar*8*pi()) = creates an undulating wave Composite Curve Trajectory Function trajpar_of_pnt trajpar_of_pnt("trajname", "pointname") The trajectory parameter of a composite curve, trajpar_of_pnt, can be used in relations. The following function returns a value between 0.0 and 1.0:   =   Logical Functions True* true() true True function Returns "YES" (For some reason doesn't return "True"!) True() True = = YES TRUE Logical Functions Yes* yes() yes Yes function Returns "Yes" Yes() Yes = = YES TRUE     *Relations containing conditional statements are not sorted. A condition is an expression that is either TRUE (or YES) or FALSE (or NO). These values can be used interchangeably in the conditional statement. For example, the following statements can all be evaluated the same way: From <https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/fundamentals/fundamentals/Conditional_Statements_in_Relations.html>     Pro/ENGINEER, Creo Elements/Pro and Creo Parametric

Workflow for creating a 2D repeat region to display family table information.  Covers an alternate method using simple repeat regions to allow the use of relations and filters.  Discusses creation of filters in alternate method, and some related drawing setup options are also covered in addition to column sorting to match the family table display order.    

Our weekly Did You Know series focuses on providing users with informative, “how-to” tips to help them get the most out of PTC Creo. This week’s post, provided by Director of Product Management Paul Sagar, shows users how to create family tables in PTC Creo Parametric. Users will learn how family tables enable you to create a large number of common parts quickly, based upon a generic design model.   Family tables are a collection of parts or assemblies which are similar, but deviate slightly in some aspect – such as size or included features. Bolts are a common example because they look similar and perform the same function regardless of their properties. It’s helpful to think of them as a family of part models. Parts in family tables are also known as table driven parts. In PTC Creo Parametric, you can create family tables in three easy steps.   Step 1: Identify Features Which Will Vary First, you must identify which dimensions or features will vary for your family of parts. Click on the Model Intent overflow menu and select Switch Symbols. This will show you the symbolic name of the features dimensions in your generic part (such as size or depth). From here, you will know which dimension will be altered in your family of parts. Click on the Switch Symbols command under the Model Intent drop down to understand the names of the dimensions in your part. This will help you identify what you need to change.     Step 2: Create the Family Table Go back into the Model Intent overflow and select Family Table. Click Add Columns in the family table dialog box. With Dimension selected in the Add Item section, click on a feature in the model, and then select the dimension you wish to add to the family table. From the Family table command, we can choose which parameters we want to alter in each of the instances we create.   We can also add parameters into our family table (such as descriptions). In the Add Items section, click Parameter, then choose what you want to add (description for instance), and click Insert Selected. You can see the parameter has been added to the table.  Parameters added to the table can be edited in each of the part instances. You can also add features from the model tree, which can be included or excluded in the part instances.   Step 3: Edit Instances After choosing the parameters, we can chose the number of instances we want in our family table. Simply click Add Instances until you have the desired quantity.  You can edit the parameters for each specific instance. To finish the table, click Verify instances. This will tell you if your changes can be regenerated. Finally, you can preview or open each instance by selecting the appropriate row and picking Open. In the family table menu you can edit and verify the specifications on each instance you will create. You can also preview each part.   In the family table menu you can edit and verify the specifications on each instance you will create. You can also preview each part.   In conclusion, family tables give you an easy systematic approach to creating a large number of related models.   Check out our video tutorial on the PTC University Learning Exchange (“Creating a Family Table”) to see this advice in action. We’d also love to hear your suggestions for working with family tables in PTC Creo Parametric.   For more in-depth product feature explanations, visit our Tech Tips area.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback! In case you missed it, here are our recent Did You Know posts: 1)    Tips and Tricks for Cable Design in PTC Creo Parametric Piping and Cabling Extension 2)    Creating Helical Sweeps for Springs 3)    How to Use Motion Skeletons to Quickly Design Mechanisms

Our weekly Did You Know series focuses on providing users with informative, “how-to” tips to help them get the most out of PTC Creo. This week’s short post shows users how to create a square to round blend in PTC Creo Parametric, the source of inspiration for this tutorial originally came from a member of our PTC Creo Community. Users will learn how to create the blend in 3 steps.   Step 1: Sketch a Square Section You have two options when creating a blend; you can either sketch the sections ahead of time and select them in the blend tool, or you can sketch the sections within the tool as you create the blend. In this example, you will create external sections and select them in the Blend tool.   Begin by creating a square section on your first sketch plane with the Center Rectangle tool in Sketcher. Sketch a Square Section     Step 2: Sketch a Circular Section and Divide it Create a second sketch plane offset from the one on which you sketched your square section. Sketch a circle on this sketch plane using the same center that you used for your center rectangle.   Each section of the blend must have the same number of entities. You will tell PTC Creo how to blend the two sections together by splitting the circle into four segments to match the four segments of the square section.   First, orient the sketching plane parallel to the screen with the Sketch View button. You will see the square section and the circular section together. Next, select the References command and select the corners of the square section as references for the sketch. Then create two centerlines diagonally across the square through the corner references, and use the Divide tool to split the circle where it is intersected by the centerlines. Divide the square and circle into an equal number of segments. This allows you to create the blend.     Step 3: Create the blend. Create a blend with the Blend tool. Select “Selected Sections” under the Sections panel. Select the rectangular section as Section 1, then Insert, then the circular section as Section 2. If the blend is twisted, you can adjust the start point of either section by selecting the section in the collector and then dragging the vertex around the section. Here is an example of what the blend looks like:   The final product: A square to round blend   In conclusion, creating a square to round blend in PTC Creo Parametric can be accomplished in a few easy steps. Check out our video tutorial on the PTC University Learning Exchange (“Creating a Square to Round Blend in PTC Creo Parametric 2.0”) to see this advice in action. We’d also love to hear your suggestions for working with blends in PTC Creo Parametric.   For more in-depth product feature explanations, visit our Tech Tips area. Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback! In case you missed it, here are our recent Did You Know posts: 1) How to Create a Family Table   2) Tips and Tricks for Cable Design in PTC Creo Parametric Piping and Cabling Extension 3) Creating Helical Sweeps for Springs

How to change the license file in FlexNet Admin License Server 11.10.0 How to reconfigure FlexNet Admin License Server with an updated license file How to reconfigure the license manager with a new license file How to update the license server (lmadmin) to point to a new license file Error "(-12):Invalid returned data from license server system" when executing ptcstatus.bat in Flexnet Admin License Server How to update application with a new license file if license server is FlexNet Admin License Server (lmadmin) The client software does not recognize the new license file. Unable to find ptcsetup.bat to update the new license

Generate a set of Creo 3D models, parts list, drawings and 3D visualization with MS Excel and PTC Creo.      

Covers creation of repeat region relations to control quantity for bulk items in an assembly BOM table.      

This week’s Did You Know, provided by our Director of Product Management Paul Sagar, teaches users how to create helical sweeps for springs using the sweep tool in PTC Creo Parametric. With this tool and its dashboard interface, creating springs is quick and easy. Paul shows us how to do so in three easy steps:   Step 1: Start Sketching the Spring’s Profile The helical sweep tool is located in the Shapes group of the modeling tab, under the Sweep Type drop down.   The sweep type drop down menu     After the helical sweep dashboard opens, go into the References tab and click Define to begin sketching the profile of the spring.   In this example, we’re going to sketch the spring’s profile on the FRONT datum plane in a 2D orientation.   Step 2: Define Spring Properties First, define the spring center line. This will be the center axis of the spring (the axis of revolution).     Defining the axis of revolution on the center line   Next, add a vertical line to the left of the center line to represent the profile of the spring. This will be the diameter of the spring defined through the center of the spring’s wire. Complete the profile sketch.   Now define the Helix section by choosing Create or Edit Sweep Section in the dashboard.   The diameter of the wire will be sketched at the start point of the profile, using a circle. But you can use any shape you need.   Step 3: Add Relations   The helical sweep dashboard makes it easy to edit the pitch value of the spring, or toggle the spring from a right hand to left hand turn. The finished helical sweep will be seen dynamically on the screen. Complete the feature.   To finish the spring however, we want to make sure the spring maintains six coils no matter how much it’s expanded or compressed. To do this, we’ll need to add a relation to the part.     Adding relations to ensure this spring has six coils     This relation will be used to control the spring’s pitch as it expands and contracts. Go to the Tools tab and open the Relations Dialog box. We can see that the height of the spring is D1, the pitch is D2, and the diameter is D0. We need to write a relation that says the pitch equals the height of the profile divided by 6. This will ensure that the spring always has 6 coils. Now we can test it by editing the height dimension to compress and expand the spring. The final product: We can continue to compress and expand the spring without changing the number of coils     Check out our video tutorial on the PTC University Learning Exchange (“Creating Helical Sweeps for Springs”) to see this advice in action. We’d also love to hear your suggestions for working with helical sweeps below.   For more in-depth product feature explanations, visit our Tech Tips area.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!   In case you missed it, here are our recent Did You Know posts: 1) How to Use Motion Skeletons to Quickly Design Mechanisms 2) Tips for Fewer Model Failures with Intent References 3) Tips for Creating Advanced Round Geometry in PTC Creo Parametric

We’re happy to announce the first edition of our “Did You Know?” series here on the PTC Creo Community, providing you with informative, “how-to” tips to help our members get the most out of PTC Creo Parametric.   Today we’re sharing three expert tips, provided by our Director of Product Management  Paul Sagar, on creating advanced round geometry inside PTC Creo Parametric:   Putting a Round on 3 Edges – You can control the specific geometry at the transition of 3 edges.  Go to the main dashboard and click on the “Pieces” menu. From here you can hover over each individual piece and the software will highlight the geometry created. You can “include” or “exclude” specific pieces to control the overall geometry. See Image 1 below: Image 1: Rounds on 3 edges   Creating a Blended Transition Between two different rounds – By default, when you select an edge it automatically rounds the tangent chain. By holding shift, you can create a round on just one specific edge. The transition between each edge is automatically blended. See Image 2 below:   Image 2: Blended transition   How to Make a Round Disappear - You can make rounds disappear into a single vertex. Go back to the “Pieces” menu and click on the single piece. This will create a drag handle. By selecting the drag handle and moving it down, you will cause it to automatically snap into the next transition. This allows you the ability to create surface-to-surface rounds, edge-to-surface rounds, or edge-to-edge rounds. See Image 3 below:             Image 3: Rounds disappear   Check out our video tutorial on the PTC University Learning Exchange ("Round Tips") to see these tips in action. We'd also love to hear your tips for creating rounds in PTC Creo Parametric in the comments below.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment and we’ll write up the best ones from the community. Thanks for reading and I look forward to all of your feedback!

PTC is pleased to announce the Creo Community Challenge, a recurring event where you can solve an open-ended challenge using Creo. Click to learn more.

Today, we’re launching the Creo edition of the PTC Community Spotlights which launched last month in the ThingWorx Community.    Here’s where we have a chance to learn a bit more about our most active community members:  who they are, the products they use, and what they like about being a member of the PTC Community.  I, Ruth Morss, am your guest host on this Creo Parametric Tips board.  Normally, I write Creo product collateral, but when Cat and Jaime Lee gave me the chance to get to know a community member, I grabbed it.   The first community member in our Creo Community spotlight series is Thom Braxton who goes by the handle @tbraxton.  He is most active on the Creo Parametric 3D Part & Assembly Design Forum.   Thom has been a member of the PTC/USER industrial design and surfacing technical committee  through 2002 and got involved again in 2019 to have the chance to influence Creo’s development. This TC is responsible for core surfacing, ISDX, Freestyle and ReStyle tools.  He currently maintains the list of open issues for core surfacing functionality.   Above, Thom enjoys his favorite hobby – cycling.  Grand Traverse trail in Vail, CO   The first non-Creo thing to know about @tbraxton is that he’s a native Floridian.  He swears you can get used to the heat but not the humidity.  Not surprisingly he enjoys the outdoors whether it’s the earth or the ocean.  One caveat: Assume any body of water has a gator in it. “Alligators invade any body of water they can swim in. There are tons of them!”    He started using Creo back in the mid-90s in its Pro/Engineer days.  He enjoys turning to the Community when he’s got a detailed technical question.  “We’ve got community members who are invaluable resources and happy to respond to questions.”     Professionally, he used to run R&D groups at Motorola – thus the magazine cover highlighting his article ‘Mapping Your Good Intentions’.  He now works as a consultant on products from medical devices to sporting goods to consumer electronics and even high-end chronometers.    A good day for him is working with people who are not technical by nature to define a problem to be solved – and then working to solve that novel technical problem. “I love the flexibility and the range of projects.  I’d get bored quickly if I were working on the same thing for my entire career.”   He continues to provide engineering and design support to a leading manufacturer of respiratory personal protective equipment (PPE). It is satisfying to see product designed and manufactured in the USA being used to fight the effects of COVID-19 globally.  Pro/E and Creo were integral to the development and manufacturing of these products.   On his wish list?  Economical 3D metal printing suitable for mass market production parts. He said Motorola had one of the first 3D printers sold commercially in the early 90s and so he had the chance to work with the technology just out of college.  “It’s evolved. It’s cool – but it’s not quite there for production parts in most applications.”           

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How to apply a torsional moment load, or torque, to a model using solid elements.  

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Our weekly Did You Know series focuses on providing users with informative, “how-to” tips to help them get the most out of PTC Creo. This week’s post, provided by Product Management Director Jim Barrett-Smith, is a brief, introductory overview of routing cables inside the PTC Creo Parametric Piping and Cabling Extension. Users will learn how to filter logical cables, add locations to axis, and understand how the next location in a wire segment will be created. Tip 1: Filtering Logical Cables First, select Route Cables under the Cabling section of the user interface. In the Route Cables dialog you will notice there is a Find tool. This will find all the wires and cables with logical references. If this is a very large list, you can refine it by simply selecting a designated component from the graphics area. When you select a designated component, the wires that attach to it are added to the Route Cables dialog. If you hold control and left click, you can select multiple components     When selecting individual components, the wires which attach to them are automatically added to the Route cables dialog   Tip 2: Adding Locations to an Axis After you place your simple route, you can start adding locations. In Pro/ENGINEER Wildfire 4.0, the system would automatically place a location onto each end of the axis. If the axis was very short, the cable would form loops in order to satisfy the minimum bend radius.     In PTC Creo, the default behavior is to add a location on the axis at the selection point. If you want the old Pro/ENGINEER Wildfire 4.0 behavior you can right click and choose  Along or you can change the configuration option default_cable_axis_location  from On to Along and the system will then place a location at each end of the axis. Note: The configuration option is from PTC Creo 2.0 M090 onwards.   When adding locations to an axis, you can revert back to the old Pro/ENGINEER Wildfire 4.0 behavior by right clicking and selecting Along. This places locations at each end of the axis.     Tip 3: Choosing Next Locations When you’re adding locations, take notice that half of the wire is orange while the other half is red. The red segments are where you’re going to add your next location. When you choose the next location and click, you’ll see that it has been added in the red segment.  If you want to add a location in the orange segment then simply choose Reverse Direction from Location tab. When choosing your next location, follow the red segments. When you choose the next location and click, it will be added to the red segment.   Check out our video tutorial on the PTC University Learning Exchange (“Cabling Design Routing Cables Tips and Tricks”) to see this advice in action. We’d also love to hear your suggestions for working with cables in PTC Creo Parametric Piping and Cabling. For more in-depth product feature explanations, visit our Tech Tips area. Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!   In case you missed it, here are our recent Did You Know posts:   1)    Creating Helical Sweeps for Springs 2)    How to Use Motion Skeletons to Quickly Design Mechanisms 3)    Tips for Fewer Model Failures with Intent References

With the release of PTC Creo 3.0, PTC Creo Parametric users now have access to an expanded library of standard parts and fasteners as well as an intuitive user interface to speed up the process of adding hardware to your assembly design. Jim Barrett Smith, Product Manager at PTC, gives an overview of the new capabilities:   To define the position of a fastener, select the datum point, axis, or a hole. You can select two aligning surfaces to define a fastener connection with a thread. Or, you can select two opposing surfaces to define a fastener and nut connection.   Next, select a fastener from the comprehensive library of fasteners. Choose the size of the thread or measure the thread size using an existing hole.     Selecting a fastener from the standard parts library   You have the option to set the length of the fastener yourself, or to have it set automatically. You can also control the hole tolerance and choose whether to have a counterbore on the top, the bottom, or both.   Setting the length of the fastener     There is a 2D preview in the dialog which updates with as you define the fastener details. Furthermore, you can click Preview to see a 3D view of the fastener in the graphics area.   You can get a 3D view of the fastener by selecting Preview     When you are satisfied, click OK to assemble the fastener.   After a fastener is assembled, you have the ability to reassemble or redefine it. Furthermore, if you reassemble an existing fastener onto a pattern, you will have the option to pattern the fastener. This saves significant time and effort.  If needed, you can choose to delete all patterned fasteners by simply selecting one and clicking Delete.     Check out our video tutorial on the PTC University Learning Exchange (“PTC Creo Intelligent Fastener (Lite)”) to learn more. Stay tuned to our “Did You Know” blog series as we cover all of the exciting, new enhancements in PTC Creo 3.0.     For more in-depth product feature explanations, visit our Tech Tips area.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!   In case you missed it, check out our recent Did You Know posts covering PTC Creo 3.0 enhancements: Flexible Pattern Tool in the PTC Creo Flexible Modeling Extension Aligning Freestyle Geometry  

The first edition of our new “Did You Know” series featured advice for creating advanced round geometry in PTC Creo Parametric. This week Don Breda, Product Manager at PTC, shows us how to use intent references in PTC Creo Parametric to avoid model failures.   Here is the situation we are trying to avoid: let’s say you are trying to change a square interface into a hexagonal interface. You redefine the extrusion and delete the square. Now, the system says you are deleting entities that are referenced by other features. Hence, we’re left with feature failures. In this particular instance both a draft and round have failed when we changed the section that is used to define the extrusion.   What causes this failure? Both the draft and round were referenced to the individual surfaces and edges of the extrusion.   How do I avoid this problem? Change the way these features are created by using intent references.   Edit the Definition of the Draft feature, and remove the individual surface references. Next, “query select” by clicking the right mouse button until all the sides of the extrusion are pre-selected - the tooltip will say IntentSrf. Click the left mouse button to select the intent reference. Instead of picking geometry explicitly to reference, you are telling the system to reference the surfaces of the sides created by the extrusion. This is the intent reference.   After editing the definition of the draft feature so that it uses intent references to always reference the side surfaces of the extrusion, we can make changes to the extrusion’s section without problems.   We can also use intent references to redefine the rounds, removing references to explicit geometry, and substituting intent edges at the end of the extrude feature.   The draft and round features no longer reference the individual surfaces and edges of the extrude feature. Instead, the draft uses an intent reference that consists of all side surfaces of the extrude, while the round feature uses an intent reference that consists of all edges at the end of the extrude. Now we can go ahead and delete the square interface and replace it with the hexagonal interface.   With Intent References, we’re able to delete the square interface and replace it with a hexagonal interface without failures occurring.   This time everything has updated properly. The draft is applied to the side surfaces of the extrude, while the rounds are applied to the end profile of the extrude.   The bottom line is whatever we change the profile to, we’ve ensured the draft and rounds will be created properly.   Check out our video tutorial on the PTC University Learning Exchange (“Intent References”) to see this advice in action. We’d also love to hear your suggestions for working with intent references below.   For more in-depth product feature explanations, visit our Tech Tips area.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!

Workflow for creating an assembly process animation video using an explode state in Creo Parametric  

PTC Creo 3.0 introduces a new Align capability within Freestyle which allows PTC Creo Parametric users to create and drive freeform, stylized designs parametrically. Users can now connect their Freestyle geometry to other external geometry with positional, tangent, or normal conditions. Furthermore, any change made to this external geometry will be reflected in the Freestyle geometry during regeneration.   Paul Sagar, Director of Product Management, gives us an introductory overview of the new Align feature:   PTC Creo 3.0 introduces a new “Align” feature within Freestyle. With this capability, you can align the freestyle control mesh to external curves and edges and therefore parametrically control your freestyle geometry.   In this example, we will be working on a bike model and building the surfaces around the pedal. These surfaces are defined parametrically by the neighboring geometry. We will start with a sphere, and build out the geometry to get it close to the neighboring surfaces.   Building out geometry with Freestyle, it will be defined parametrically by the neighboring geometry     In this case, the part is symmetrical, so we are able to mirror it.   Next, you can select the faces you want to delete and leave open. You can then take the edges of the open loops and align them to the edges of the neighboring geometry.     Aligning the edges of the part to the neighboring geometry     After the loops and edges are aligned, you can specify the continuity between the Freestyle geometry and the surrounding geometry. In this example, we will create a normal connection.   While we continue to refine the shape, we need to define the location for the pedals. Again, when the geometry is close, you can align the external edges of the geometry.   Here is a look at the completed geometry:   A look at the final geometry     Finally, you can return to the top level assembly and make changes to the skeleton model that is driving the shape of the frame. When regenerated, the Freestyle geometry is also updated to maintain the connection and tangency to the surrounding geometry.     Changes to the skeleton model will be automatically reflected in the Freestyle model during regeneration     In conclusion, with the new Align capability you will be able to more effectively combine freeform, organic geometry with dimension based design intent.       Check out our video tutorial on the PTC University Learning Exchange (“Aligning Freestyle Geometry”) to learn more.   Stay tuned to our “Did You Know” blog series as we cover all of the exciting, new enhancements in PTC Creo 3.0. For more in-depth product feature explanations, visit our Tech Tips area.   Have some ideas about what PTC Creo product features you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!