Drawing Formats And Templates CREO - Community.ptc
Creotm ParametricEducation Advanced EditionDrawing formats and templates02Drawing formats and templatesC1-SE-L1-J.E.F-10
Written by These materials are 2010, John ForthJohn ForthAmended Dec2008 for Creotm ParametricAll rights reserved under copyright laws of theUnited Kingdom, United States and othercountries. Amended 2010 for Creotm ParametricPTC,thePTCLogo,Pro ENGINEER,Pro DESKTOP, Wildfire, Windchill, and all PTCproduct names and logos are trademarks orregistered trademarks of PTC and/or itssubsidiaries in the United States and in othercountries.Conditions of use Copying and use of these materials is authorisedonly in the schools colleges and universities ofteachers who are authorised to teach CreotmParametric in the classroom.All other use is prohibited unless writtenpermission is obtained from the copyright holder.AcknowledgementsManufacturing Proofing and comments –Trialling materials Feedback In order to ensure these materials are of thehighest quality, users are asked to report errors tothe author.JohnF@dteconsultancy.plus.comSuggestions for improvements and other activitieswould also be very welcome.C1-SE-L1-J.E.F.-10
ContentsDrawing formats and templates .1Creotm Parametric Schools and Schools Advanced Edition.1Contents .3Overview.5To assign a dtl file to the config.pro file .7About Drawings.9Detailed Drawings Module.10Create a New Drawing .11Adding Dimensions .14Adding new sheets.19Pictorial Views.20Creating a sectional view .21Sectional View Created in the Drawing file .24Enlarged Details.25Offset or Stepped Section .26Modifying Cross-Hatching display.30Exploded Views .32Other Views .32To create a customised exploded view .33More with Annotation. .35To Change the Format Sheet.37To Create your own Format.38To add a Table.43To Add a Logo .46DTE Consultancy3
To Create a Template.49To Add a Bill of Materials (BOM) Table.51Creating a Bill of Materials for a blank format. .54Creating the BOM for an assembly .54To create a new Repeat Regions Table.58Appendix 1. Setting up and editing a Drawing Options File. .63Appendix 2 System Parameters for Drawings .65Appendix 3: To Control the Format of the Date .69Appendix 4. To create a multiple parts drawing.70DTE Consultancy4
OverviewThe creation of an Orthographic set of drawings in Creotm Parametric is very simpleonce you get the hang of it but can appear daunting when you first approach theprocedure.The first thing you have to keep in mind is that what you are creating is a particular wayof looking at a three dimensional object.In the diagram below you can see the relationship between various aspects of theoutputs available from Creotm Parametric. The various part models (*.prt) can beassembled to form complex assemblies (*.asm). Both parts and assemblies can beshown as drawings (*.drw). Whilst not part of this tutorial, the models can also beshown as rendered images; simulations and animations; and behavioural models usingthe Finite Element Analysis (FEA) part of the Schools Advanced ering drawing(s)ComponentsEngineering drawing(s)3D AssemblyRendered Image(s)AssembliesSimulations and AnimationsBehavioural Models (FEA)For Orthographic drawings, often called Detail Drawings, Creotm Parametric merelyrepresents this 3D object using whatever standard you have chosen.The diagram below summarises the relationship between the 3D model or assembly;the engineering drawings and the various ways that the program creates the drawingsand sets the agreed standards for that particular set of orthographic drawings.DTE Consultancy5
3D ModelConfig.proor ngineering drawing(s)FormatTemplate.dtlTemplateBOM Blank tableFirstly, make sure you have the correct drawing setup file (*.dtl) referenced in theconfig.pro file. The standard ‘look’ of orthographic drawings will vary depending on thepart of the world you are in and which particular set of standards you need to use tocommunicate your ideas with others. In the United Kingdom the British StandardsInstitute set the agreed standard, the current one for schools being BS8888. In otherareas the ISO (International Organization for Standardization) or ANSI (AmericanNational Standards Institute) standards apply; if you work in these areas you will needto set the Configuration File to suit your standard.In Creotm Parametric there are a number of batch files (*.bat) in the ‘pro standards’folder of the program. Activating the appropriate batch file will set the config.pro file tothe correct standard for your needs.To create a drawing you will also need a Format, this file is the ‘look’ of your drawings.The Format can also be overlain with a Template that positions the views and createsthe text height, line type etc. This is controlled by the *.dtl file which could be the default,in this case the bs8888.dtl file, or a specially created one called the Active Drawing Filewhich will only affect the drawing to which it is attached. If a Bill of Materials (BOM) isrequired, a ‘bom’ table can be inserted into the Template that can extract the necessaryinformation from the Bill of Materials contained within the assembly file. A drawing format file (*.dtl) can be tailored to a specific set of drawings and savedunder a name, e.g. Oil Box.dtl in which special changes are made to suit the needsof this set of drawing. This is the Active Drawing file. If a Template is used its drawing format file (*.dtl) file will determine the outcomesunless overwritten by an Active Drawing file. If no template is used then the Global dtl file, e.g. bs8888.dtl, will be used.DTE Consultancy6
To assign a dtl file to the config.pro file1. Open the creo standards folder in the C:/Program Files/PTC/ Creo1.0/CommonFiles/F000. It will look a little like the one above. Read the README.txt file therein(reproduced below)Dear Creo Users,The PTC Education Group has provided a number of batch files to helpset your default units quickly and easily.If you choose the "Metric" option during the installation of CreoParametric, it is installed usingthe MMKS Unit System and ASME drawing standard.If you choose the "English" option, Creo is installed using theINLBS Unit System and ASME drawing standard.You can easily reconfigure your installation to follow a differentUnit System and/or Drawing Standardusing one of the supplied configuration .bat files as follows:1) Exit Creo Parametric.DTE Consultancy7
2) Double-click one of the five ".bat" files to configure yourPro/ENGINEER Education installation for a desiredUnit System and Drawing Standard:unitunitunitunitthisconfigure for asme inlbs.bat – ASME standard drawings with INLBSsystemconfigure for asme mmks.bat – ASME standard drawings with MMKSsystemconfigure for bs mmks.bat – BS8888 standard drawings and an MMKSsystemconfigure for iso mmks.bat – ISO standard drawings and an MMKSsystem (1st Angle Projection & Commas)configure for STANDARD UNIT-SYSTEM.bat - For advanced users only,can be edited to create your own custom setup.3) Restart Creo*** Notes:1) To configure your installation using the supplied .bat files, youmust have read/write access to the yourCreo loadpoint folder (and subfolders). This folder is typically"PTC".In Windows 7 and Vista, this typically requires you to disable theUAC (User Account Control) and restart your computer.2) Prior to running a configuration .bat file, you will see drawingtemplates for BOTH MMKS-ASME (A1,A2,A3,etc)and INLBS-ASME (A,B,C,etc) drawing templates. You should only usethe templates that are relevant to yourunit systems.3) The following folders contain drawing standard specific DrawingTemplates:templates asme in – Inch length unit, ASME standard drawingtemplates, Sizes A,B,C&D.templates asme mm – MM length unit, ASME standard drawingtemplates, Sizes A1,A2,A3,A4.templates bs mm – MM length unit, BS8888 standard drawingtemplates, Sizes A1,A2,A3,A4.templates iso mm – MM length unit, ISO standard drawingtemplates, Sizes A1,A2,A3,A4.(1st ANGLE PROJECTION).In my case I have activated the one in bold above2. Double Left-Click the appropriate batch file.3. Now when you start the program the relevant standard is set.If you want to use the default set of Formats and Templates then this is all you need doto set things up. However if you notice some anomalies in your drawings then you mayhave to edit the *.dtl file, to do so see Appendix 1.DTE Consultancy8
Above is an example of a Drawing Setup File (*.dtl).About DrawingsUsing the Creotm Parametric Drawing mode, you can create drawings of all models, orimport drawing files from other systems. You can annotate the drawing with notes,manipulate the dimensions, and use layers to manage the display of different items. Allviews in the drawing are associative: if you change a dimensional value in one view,Creotm Parametric updates other drawing views accordingly1. Moreover, CreotmParametric associates drawings with their parent models. The model automaticallyreflects any dimensional changes that you make to a drawing. In addition,corresponding drawings also reflect any changes that you make to a model (such as theaddition or deletion of features and dimensional changes) in Part, Sheetmetal,Assembly, or Manufacturing modes.1Only those parametric dimensions used to create the 3D model can do this. Extra dimensions addedmanually cannot.DTE Consultancy9
Detailed Drawings ModuleDetailed Drawings extends the drawing capability of Drawing mode. You can use it withCreotm Parametric to create, view, and annotate models and drawings.Detailed Drawings support additional view types and multisheets, offers numerouscommands for manipulating items in a drawing, and lets you add and modify differentkinds of textual and symbolic information. In addition, you can use it to customizeengineering drawings with sketched geometry, create custom drawing formats, andmake multiple cosmetic changes to drawings.With Detailed Drawings, you can also use a shortcut menu to modify any object in adrawing from anywhere in the model tree. At any time when a drawing window isactive, you can interrupt your current process and activate a drawing object formodification.With Creotm Parametric Interface or Detailed Drawings, you can access variousinterface commands for exporting drawing files to other systems and importing files intodrawing mode.To understand the views you can get from your model or assembly, in your 3D model,use the Saved Views ; here you can set Front, Top, Left, Right, Trimetric andIsometric views plus a few others. Try it now, in the modelling mode; alter the model toNo Hidden, (Left-Click ) as you do so. You will soon see how Orthographic and 3Dviews are related in Creo ParametricAbove is the LEFT view, to the right isthe FRONT view and below is theTOP view. Note how one relates tothe other. The datum planes on showshould help you understand this.DTE Consultancy10
Create a New DrawingWith a 3D model open on the screen1.Left-Click File then click New2.Select the ‘Drawing’ radio button3.Type in a name for your drawing file4.Make sure the ‘Use default template’box is ticked.5.Left-Click6.Pick the drawing size you want andLeft-ClickDepending on the part or assembly you have open on the screen; the design of theformat and template you use, you will now get the 2D drafted representation yourequire. It will not be complete but of that later.(Note: If you have Datum planesand Coordinate systemsopen to view then theywill appear in the drawing. Just turn them off and Left-Click anywhere in the Graphicswindow to see them disappear or Left-Click repaintDTE Consultancyor Ctrl R )11
If you look at the picture above you will see what is meant. There are certain elementsmissing; i.e. dimensions and some elements may be wrong for your standard; therepresentation of the filleted corners for example. Note the blue line (pre-selectionhighlight) around the view that will help us change things. Note also such things as theborder around the edge, the folding guides and reference numbers, the text boxes etc.This is known as the Format and you can create your own format. The three viewshaven’t appeared by magic. Their position and appearance is due to another file thatoverlays the format and is called the Template. It is the combination of your model, theformat and template that makes the drawing unique (see diagram on the next page).First take a close look at the screen shot and note that it has a new feature, this iscalled the Ribbon Interface.Each tab on the ribbon allows different options into play. Left-Click each tab and notethe Commands that appear that also appear in other ribbons. Right-Click in the graphicsare and note the commands available for rapid use.DTE Consultancy12
Select each drawing tab to observe the functionality found in each: Layout – Sheets, formats, views, display settings and drawingobjects are controlled from this tab. Table – Tables are created and edited using tools in this tab. Annotate – Dimensions, notes and tolerances are shown, createdand controlled using tools in this tab. Sketch – 2D draft entities can be sketched using tools in this tab. Legacy Migration – Take old models and those from other software Analysis – Similar to the analysis ribbon in the modeling mode. Review – Update your drawing, compare different versions, queryfor information and take measurements using tools in this tab. Tools – Various drafting tool and access to the template creation mode. View – Tools to change the view parameters.As we progress through the tutorial these features will be addressed in more detail.Relationship of model and drawingsThis is the model, it appears in the finalsheet which is made up of the format;the template that places the views andfinally the drawing with the views inplace.7.Double Left-Click on the blue line, it goes red indicating selection, the followingdialogue box appears, the use of this will allow you to modify the views.Note: The list of categories down the lefthand side.8.Left-Click each and see what youget.9.You can play about with the optionsand if you Left-Click thebutton you can see how the viewchanges; if you don’t like it change itback.DTE Consultancy13
The important one at this stage is theView Display. Here we can show or hideHidden lines and remove tangent edgedisplay. On our own templates, createdlater, we can automatically set thesefunctions.10. If you want to show hidden lines andno tangent edges then choose asshown here.11. Once you have finished Left-ClickorthenAdding Dimensions1.Select the view that you wantto add dimensions. Left-Clickthe Annotations Tab in theRibbon Inteface.Left-Click theblue line, you will find it byfloating the mouse near to theview.2.Left-Click Show ModelAnnotationsand thefollowing floating menu willappear.3.Left-Click Show All Dimensions.Don’t panic, I know there are alot and they are in the wrongplaces. We will proceed toedit their position and removethe unwanted.4.Left-Click OK5.If you select the view againand Right-Click; In the FloatingMenu you will see the optionto Cleanup Dimensions. Thisallows you to quickly movethings about so you can seethe wood from the trees.DTE Consultancy14
The Offset is for the first dimension anddefaults to 12.5mm, each subsequent(Increment) dimension is 5mm on fromthe offset. A set of dotted guide lines isshown to help set them up. These canbe deleted as explained below. To notshow them uncheck the Create SnapLines boxFor the moment just accept the defaults6.Left-Click7.Now Left-click to select and Delete all the hatched guide lines; (Use the Ctrlkey to select multiple lines and then hit the Delete Key (see drawing above)DTE Consultancy15
8.Now select those dimensions you want to delete, either one at a time ormultiple select using the Ctrl Key select with a Left-Click then Right-Clickand select Erase. (If you hit the Delete key they will disappear immediately)The dimension(s) will grey out and only disappear when you select the next one oranywhere in the Graphics Window. This gives you the opportunity to Right-Click andUnerase if you accidentally choose the wrong one. Whilst you are doing this you canalso Left-Click-Drag to reposition the dimension and/or the value.9.Spend some time ‘tidying up’.10. In Creotm Parametricyou can move a dimension from one view to another. Theprocedure is very simple.a. Select the dimension to move with a Left-Clickb. Right-Click and select Move item to viewc. Select the view to receive the dimension. Note: It has to be one that hasthe feature orientation that is suitable.11. You can add a note to a dimensionvalue by Double Left-Click the valueand follow the instructions in thedialogue that appears. As shown hereYou can alter a lot of things on these threeboxes to determine exactly what you want. Inthis example we have added the prefix “4 X” tothe Ø@D. (This is the code for the Ø5mm of thefour mounting holes.) This is neater thandimensioning each one.Your view will now look a bit like this.DTE Consultancy16
12. You can now manually adddimension using the sametechnique as in theSketcher.13. Select the Create StandardDimensionTool from theToolbar14. Also Align Dimensions.First selected will be thedatum. Other will align to it.15. Left-Click to select the firstobject of the dimension;edge, axis, etc., Left-Clickthe second object.DTE Consultancy17
16. Then Middle-Click whereyou want the dimensionplaced.Note: These added dimensions arenot parametric and will not changethe model if you try to change them inthe drawing.17. To add Centre Lines (Axis)Left-Click the view on whichthey are to be placed.18. Left-ClickAxis Tab.and select the19. Put a check in the box ofthe Axis you want, or selectall.20. Left-ClickDTE Consultancy18
Notes can be added as can a Bill of Material (BOM) table and much more. If you wantto use this function see the section To Add a Bill of Materials (BOM) Table.Remember that these apparent drawings are in fact representations of 3D objects andassemblies. As such any changes made to them will be reflected in these drawings.This Associativity is an important productivity aspect of Creotm Parametric. You can tryit by opening the part,1. (Right-Click in the Navigation window on the part and choose Open),2. Change a feature of the part or add an extra chamfer. Now go back to the drawingand see that the change has already been made.3.In some cases you may need to regenerate. Left-Clickthe drawing. This is theessential difference between a 3D modelling CAD and a 2D drafting CAD.Adding new sheetsYou can add sheets to the file.1. Left-Click New Sheet on the LayoutTab. This will come in as a blankformat onto which you can placegeneral and projected views, createsections or even exploded views.DTE Consultancy19
Pictorial ViewsWhen you create your part or assembly you also can create views using the ViewManager. Also with View Manager you have the ability to set special 3D views thatbest show your model. These views can also be used within drawings.To create a special view move the model in the Graphics Window as required.1. Open the View Manager2. Left-Click Orient ,3. Left-Click New and type a name e.g.3D.4. Close the View Manager. Return to the Drawing window5. On the new blank sheet Right-Click and select from the menu Insert General View.6. Left-Click on the sheet, where you want to place the view. The drawing viewdialogue box opens to allow you to finalise the view.It opens in View Type.1. Type in a model name and then scrolldown the list of Model View Names untilyou find the one you want. Trimetric,Isometric and your own 3D views are allavailable.2. Left-Click; notice the view isshaded as it appears in the part modeller.Use other functions in the Drawing Viewdialogue to set other aspects of the viewas you desire, in the same way asdescribed previously. To set a differentscale go to the Scale category and selectCustom Scale, place a decimal numberto represent your needs, e.g. 2.0 willdouble the scale from the default.On completion Left-Clickthen.You will notice that the view is locked in place. If you want to re-position the view on thesheet you will need to select the view, (Red line around it); Right-Click and un-tick LockView Movement then Left-Click-Drag to the new position. To lock the view again, reversethe procedure. You can place more than one view on the same sheet.DTE Consultancy20
In this case the right hand view is a specially created one called 3D and it is shown withHidden detail showing. These appear as greyed out lines but will print-out or plot usingwhatever standard you have set; they appear as dashed lines in BS8888 for example.Creating a sectional viewTo create a sectional view you have to start in the part /assembly file. The simplest wayof creating a section is to make sure there is a datum plane lying just where you wantthe section to be. You can either use the ones created when the model was made oryou can place a plane with its sole purpose being to create a sectional view.You can also create a sectional view within the drawing file itself; see the sectionheaded ‘Sectional View Created in the Drawing file’. Creating the sectional view withinthe model does allow you to see the finished section and also use it to create a 3Dsectional view, something unique to 3D Modelling packages.DTE Consultancy21
1.Activate the View Manager and selectthe Xsec tab.2.Left-Click New; type a name or letterand hit return. You will be presentedwith some choices in the MenuManager.3.Accept the defaults and Left-ClickDone. The Menu Manager changes andyou have to create or select theDatum Plane you intend to use as thecutting plane.4.In the Graphics window select the plane required. You will be then back in the ViewManager.5.Left-Click Display, Select Set Active and the model will be sectioned to show how itwill appear. If you want to cut off the opposite side Left-Click Display Flip.The view will appear as below. To return tonormal viewDouble Left-Click No Cross Section.You can go on and create as manydifferent sections as you think you require.When completethe ViewManager.You can now go to the drawing view and create the sectional views you require.DTE Consultancy22
6.Create a general or projected view on the sheet, this view will be sectioned. Tocreate a projected view. Select the parent view; Right-Click and select InsertProjected View. A ghost of the view will appear Left-Click when you have positionedit. Whether it is a 3rd Angle or 1st Angle will depend on how you have set up theDrawing Options File (see Appendix 1).A.a. Select the view with aDouble Left-Click to openthe Drawing View box.b. Select the SectionsCategory7.Left-Click select the radio button2D cross-section8.Left-Click the “ ” and the availableXsec will appear. Note: Somewill obviously not be possible onsome views.9.Left-Click to select the one youwant and Left-Click. Theview will change to appear asbelow.DTE Consultancy23
Left-Click CloseSelect the view and Right-Click selectAdd Arrows and then choose the viewto which the arrows should beattached.The view will now look something likethis, see below.If the hatching is too widely spaced orat the wrong angle Double Left-Clickon the selected hatching and a MenuManager will appear that will let youchange whatever is needed to createthe right effect. The Section title canbe repositioned by Left-Click-Drag.To remove hatching from any partselect it by Double Left-Click and setthe spacing so wide that it disappears.Sectional View Created in the Drawing fileIf you have not created the sections within the model file it is still possible to create thesection from within the drawing window. Ensure you have the Datum Planes visible anda Projected view created that will be sectioned.a. Select the view with aDouble Left-Click to openthe Drawing View box.b. Select the SectionsCategoryDTE Consultancy24
At this point there will be no Xsec in the box.1. Left-Click ‘ ’ and Create New2. Select Planar Done3. Enter a Name or Letter4. In the Menu Manager Plane will be highlighted if not select it.5. In the graphic Window Left-Click the Datum plane to be used (in anassembly use a ASM datum plane, you may need to Right-Click anduse Pick from list to find the required plane) Or select from the ModelTree6. In Arrow Display select the view in which the arrows will bedisplayed.7. Left-Click OKEnlarged DetailsTo create a detail is quite easy. It is in three parts, first select the feature you want tohighlight; then create a spline curve surrounding the part; then place the detail view. If asectional detail is selected then the detail will be a section.1.Left-Click Insert DrawingView Detailed2.Left-Click to select the feature,edge or face etc. A cross willappear that indicates the centre ofthe detail.Move away from the centre cross andcreate a spline curve surrounding thedetail. (There is no need nor is itpossible to use the Sketch Spline tool )3.You do not have to complete thecurve, when you get close MiddleClick and a dashed circle willappear.DTE Consultancy25
4.Left-Click in the position you want the detailed view and it will appear. The defaultscale is 2:1(set in the *.dtl file) but Double Left-Click the scale value to enable it tobe varied.The sheet will now look like this. Dimensions can be added to detailed views.Offset or Stepped SectionThere is occasionally the need to create a sectional view that uses a set of offset linesor steps to define the section cutting plane. To do this is not difficult but requires a clearapproach to the objective.DTE Consultancy26
Here is an example of a Stepped or Offset Section, Note that lines denoting the stepsare not shown in the sectioned view, however since this is an assembly the hatchingsare separate.Follow the instructions to create a Stepped section1.Insert a general view to be theparent of the Stepped Sectionor choose an existing view.2.Right-Click and from thefloating menu select InsertProjection View and place it.3.Double Left-Click theprojected view and chooseSections from theCategories list in theDrawings View dialogue.4.Choose 2D section5.Choose6.Choose Offset Bothsides7.Choose Done and enter aletter in the dashboard area tolabel the section, hit EnterDTE ConsultancyYour sheet should look like this.27
What happens now is that a newwindow opens that is very muchlike the sketcher. Notice the faceon which we are to place thestepped line has been selected.Select the face and accept all thedefaults.8. A References window opens.9. Left-Click to select 4 edges toenclose the area on which tosketch the stepped line asshown opposite. Close thereference dialogue.10. Left-Click Sketch Line LineDTE Consultancy28
11. Sketch the stepped line as if itwhere in the sketcher startingat one of the reference edgesand finishing on anotherreference edge. Use theautomatic Horizontal andVertical Constraints, there canbe no lines at any other angle.12. This line can be dimensioned inthe same way as in thesketcher. Select Sketch Dimension Normal. Usethe Constraints tool to alignwith axis and any other featurenecessary13. To complete the line creation
Drawing formats and templates Drawing formats and templates Creotm Parametric Education Advanced Edition 02 C1-SE-L1-J.E.F-10 . Written by John Forth . Using the Creotm Parametric Drawing mode, you can create drawings of all models, or import drawing files from other systems. You can annotate the drawing with notes,
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