Create a 2D Sketch: File > New > in the dialog box > Type: Part, Sub-type: Solid, Name: enter a name > OK. The default datums will appear along with the MODEL Tab that contain the tools needed to sketch and extrude the part.

• Next, select the Sketch button > the Sketch Window appear > pick a Plane on the screen or the tree > click the Sketch button which is equivalent to OK.
• Next, the Sketch Tab will appear, here you'll find tools not only to Sketch but also to Constrain, Edit and Dimension your geometry.
• Next, create circles, boxes, and lines. To finish the geometry just click the Middle Mouse Button (MMB) and basic dimensions will appear, which you can always change by clicking on them.
• To create 3D sketches or 3D lines you can use Point features and then create lines between them: first go to MODEL > DATUMS > POINT, place the points where needed. Next, MODEL > DATUM > CURVE > Curve Through Points, select the reference points and choose between straight-lines or spline.
• DIMENSIONS: You can turn displaying dimensions On or Off by going to SKETCH Tab > Setup > Display > Dimensions | Constraint | Vertices | Grid.
• NORMAL TO SCREEN: You can work sketching in normal view by SKETCH Tab > Sketch View.
• SKETCH ORIENTATION: Go to SKETCH Tab > Set-up > Section Orientation > Set Horizontal Reference | Set Vertical Reference | Restore Section Orientation | Flip Section Orientation | Flip Sketch Plane.
• Next, when you're done with the sketch hit the OK button in the SKETCH Tab.

Creating 3D Model Part-Solid files

• Once you leave the SKETCH Tab you will be sent back to the MODEL Tab where you'll find the functions needed to create 3D geometry out of your sketch.
  
• EXTRUDE: You have the options to extrude 1) a specific distance, 2) both directions, 3) up to some feature, 4) remove material, 5) as a thin shape, 6) with a taper.
  

• SWEEP-PROTRUSION: the order of operation is to first create a trajectory and then sketch the profile to be swept along the trajectory:

  1. Insert > Sweep > Protrusion the PROTRUSION:Sweep window appears; you are given the option to sketch the sweep trajectory (Sketch Traj) or Select an existing sketch to define the trajectory (Select Traj).
  2. Select trajectory > OK > select the end point for the Start Point [Accept | Next | Quit] of the profile > Done > Free Ends > Done.
  3. You are taken to the Sketch Section to define the profile, sketch the profile > OK > to exit the sketch section.
  4. In the PROTRUSION:Sweep menu click on Preview or OK.

• SWEEP-THIN PROTRUSION: the order of operation is to first create a trajectory and then sketch the profile to be swept along the trajectory:

  1. Follow the steps for SWEEP-PROTRUSION up to step 3. Then define which way the wall thickness ought to extrude (MaterialSide) inwards, outwards or both [Flip | Okay | Both].
  2. Next, enter the Thickness... watch for the many menus that appear around the PROTRUSION:Sweep, Thin window.
  3. In the PROTRUSION:Sweep, Thin menu click on Preview or OK.

• BLEND PROTRUSION: Blend two or more profiles by toggling between each profile definition and specifying a depth between each.

  1. Insert > Blend > Protrusion the Menu Manager appears [Parallel | Rotational | General | Regular Sec | Project Sec | Select Sec | Sketch Sec | Done | Quit], select Parallel and Done.
  2. Next, the PROTRUSION: Blend window appears; also the Menu Manager window appear [Straight | Smooth | Done | Quit], click Done.
  3. Next, the SETUP PLANE sub-menu appear [Plane | Make Datum | Quit Plane], pick a plane from the screen.
  4. Next, the DIRECTION sub-menu appears [Flip | Okay], choose a direction and click "Okay".
  5. Next, the SKET VIEW sub-menu appear [Top | Bottom | Right | Left | Default | Quit], click Default.
  6. Next, you're taken to the Sketch section to draw the 1st blend profile. Then R-click > pick Toggle Section in the pop-up menu > draw a 2nd blend profile > OK to exit sketch.
  7. Next, the DEPTH sub-menu appears [Blind | Thru Next | Thru All | Thru Until | From To | Done | Quit], select Blind & click Done and "enter depth for section 2" appears, enter a depth and click OK.
  8. Preview the created blend and click OK.
  9. You can add more section profiles by toggling, drawing and adding depth between each section.

• SWEPT BLEND: this example will show the basics of blending two profiles:

  1. Create a sketch to be used as trajectory, then Insert > Swept Blend in the References tab select trajectory sketch.
  2. In the Sections tab click one end of the trajectory sketch to define the first Section Location, then click the Sketch button; then draw the first blend profile.
  3. In the Sections tab click the Insert bottom to create the second section profile; click the other end of the trajectory sketch to define the second Section Location.
  4. Create the second profile; use the Line Divide if necessary to split the sketch and match the sections of the first sketch. Then click OK.
  5. When you see the blend profile preview, try changing the tangent blends and other options, then finish with OK.
• Note that next to the MODEL Tab is the VIEW Tab: the VIEW tab provide options to change the material appearance, perspective view.
• Note that next to the MODEL Tab is the APPLICATIONS Tab: the APPLICATIONS Tab provide options to create photo-realistic rendering, change scenes and other presentation tools.
• MATERIAL, UNITS, MASS, PARAMETERS: To specify go to FILE > Properties > Model Properties.

Creating 3D Model Solid-Sheetmetal files

1. File > New > in the dialogue box > Type: pick Part, Sub-type: pick Sheetmetal, Name: enter a name > OK.
2. Next, create the base of your sheetmetal part, go to Insert > Sheetmetal Wall > Unattached > Flat... in the Reference tab Sketch click the Edit button.
3. In the sketch section define the geometry and click OK. Next, enter the sheetmetal thickness and press OK.
4. To create a Flange and other appendices to the base section go to Insert > Sheetmetal Wall > Flange

Create an Assembly (Bottom-UP style): File > New > in the dialog box > Type: Assembly, Sub-type: Design, Name: enter a name > OK. The default datums will appear along with the MODEL Tab that contain the tools needed to start the assembly.

• Next, select the Assembly button > the File Window appear > pick the part file you want to import into the assembly > click OK button.
• Next, the Component Placement Tab will appear > pick the matting features and type until the STATUS is shown as fully Constrained
• Each constrain is shown as a tag in the assembly MODEL not in the tree!!! Click the Tag to re-edit the constrain.
• Next, once the part appears in the assembly area the constraint option is set to automatic by default and if you can pick similar geometries they will be mated coincident to one another and they will be rigid.
• Next, to disable the automatic rigidity of the assembly: in the MODEL TREE Tab, click settings > Tree filter > Display: Features > Apply > OK.
• Next, R-click the part > in the pop-up menu select Edit Definition > this will return you to the Component Placement section of the assembly.
• Next, click on the sub PLACEMENT Tab and uncheck the option Allow Assumptions Fully Constrained, this will stop Creo from fully constraining the part and only count the manually placed constrains.
• Next, click the Drag Component button and try moving a part along its constraints.
• The Repeat feature allow you to copy a part and its constraints: MODEL Tab > Component section > Repeat (circle arrow icon)

Create an Assembly (Top-Down style): File > New > in the dialog box > Type: Assembly, Sub-type: Design, Name: enter a name > OK. The default datums will appear along with the MODEL Tab that contain the tools needed to start the assembly.

• Define a Skeleton Model to drive parts in assembly: MODEL Tab Component section > Create > in the CREATE COMPONENT dialog box > Type: Skeleton Model, Sub-Type: Standard, File Name: something > OK
• click on the Skeleton Icon (LMB) in the Assembly Tree and select Activate, now sketch reference geometry to drive other parts in the assembly.
• Define first component in the assembly: MODEL Tab Component section > Create > in the CREATE COMPONENT dialog box > Type: Part, Sub-Type: Solid, File Name: something > OK
• in the CREATION OPTIONS dialog box > Creation Options: Locate Default Datums > Locate Datums Method: align csys to csys > OK
• Click on the Coordinate System icon of the assembly and a new part icon is added to the design tree
• Click on the new part icon > in the pop-up menu select Activate in order to begin working on it
• Note: in order to use feaures of a non-active part as reference to create geometry in another part you must enable REFERENCES
• In the SKETCH Tab, setup section click References or press RMB for a second until a pop-up menu appears > Select: Use Edge/Offset > now you can pick the non-active geometry.
• Note: to relocate Datum Tags > press the LMB to highlight the Tag, then press RMB until a pop-up menu appear > select Move Datum Tag then pick the place on the screen where you want to relocate the Tag... weird

Create a Frame Assembly: Create a part file and draw a 3D frame structure with sketches. Next, Create an Assembly file and import the part file containing the 3D sketches.

• Got to File Tab > Options > Configuration Editor > Find > type afx_enabled in the keyword search > click the find now button > click Add/Change button, then Close. Note that the file is loaded, then Click OK.
• In the Assembly go to FRAMEWORK Tab > Profiles > New Profile > Select the Beam Profile Shape & Size needed > click Close.
• Now select to place the beam using Reference Method such as a straight-line, points, or bend curve.
• Move and Rotate the beam as needed and then click the Repeat or OK next button.
• To Edit the rotation and orientation of a beam that is already in place: Framework Tab > Profiles > Move.
• To place Basic joints between beams: Framework tab > Joints > Basic Joints > choose between mitter, corner, gap and other joint.
• To place Advanced joints between beams: Framework tab > Joints > Advanced Joints > choose between Cutout, Planar trim and other joint.

Create a 2D Drawing: File > New > Type: Drawing, Name: enter a name > OK. A New Drawing window appear > in the Default Model field click the Browse and choose a 3D model > Specify template: Use template (pre-defined for your company), Empty with format, or Empty.

• Use template > choose a standard or company provided sheet size > Ok.
• Empty with format > Format: select A, B, C, etc. size sheet or a user-defined sheet > Ok.
• Empty > Orientation: Portrait, Landscape, Variable > Size: choose a Standard Size sheet > Ok.

To insert the parent view: Layout tab [Model views] > General > choose No Combined State (unexploded) > OK > LMB click in one spot to drop the view > in the Drawing View window choose from the Model view names options (FRONT, BACK, LEFT, etc.), then View Display [Display Style] and Scale > apply > close. I do not know why they put an OK button there if they disable it after pressing apply. Tip: to skip the Select Combined State prompt check the option box for that purpose. If you choose DEFAULT ALL for an assembly drawing, the view will be exploded.

To insert projection views: Layout tab [Model views] > Projection > select the parent view and drag the new view to the desired location.

To change a view position on the page: Layout [Document] > Lock view movement > LMB click view and then drag the view to a new location. You can also R-click the view icon in the tree and pick Lock View Movement from the pop-up menu. To hide a view: Layout [Display] > Erase view > select the view and a box is shown instead. To un-hide a view: Layout [Display] > Resume View > select the box > click Done Sel in the pop-up menu. To delete a view R-click the view and select delete from the pop-up menu.

To change the scale of the sheet: double-click the SCALE shown at the bottom-left corner of the page > enter new scale number > Apply, OK

To change the scale of a view: double-click the view > Drawing View window > Category: Scale > Custom Scale > enter number > Apply, OK

To change the line display of a view: double-click the view > Drawing View window > Category: View Display > Display Style > Choose between Hidden, No Hidden, Wireframe, Shading with Edges > Apply, OK

To add views from a different part or assembly: Layout [Model Views] > Drawing Models > choose Add Model from the DWG MODELS menu > pick a model file > Open. Remember that the latest model added will become the current model and any new view created will be related to it. You can change the current model by choosing the Set Model option from the same menu. Del Model will only work if there are no views generated from the selected model. All the options available from DWG MODELS menu are:

• Add Model
• Del Model (purges a model file from the drawing, all the views must be deleted first)
• Set Model (Allow you to pick a new current model from a list of available ones)
• Remove Rep
• Set/Add Rep
• Replace
• Model Disp
• Done/Return

To create a detail view: Layout [Model views] > Detailed > click on the target spot on the drawing > click several points around the target spot > MMB to place the detail circle > LMB click the area where you would like to place the new view. Position as desired.

To create an auxiliary view: Layout [Model views] > Auxiliary > Select a reference edge > select a point (LMB) to place the new view.

To create an offset-line section (revolved) view: 2x-click the view you would like to section > in the Drawing View window > Categories: Sections > 2D cross-section > click the plus (Add cross-section to view) button > Create new > in the XSEC CREATE menu > Offset > Both Sides > Single > Done. Enter a section name (A, B, C) in the pop-up window > Ok. The model will now be displayed in a modeling window: here you must select or create a plane and sketch the section profile. Also the SETUP SK PLN is displayed. Select the plane in the modeling window > OK from the DIRECTION menu; the SKT VIEW submenu will be displayed. Choose default from this submenu. Draw the sketch using the tools in the top menu (View, Sketch). When finished: Sketch > Done. The last step is to display the section line-arrows in the drawing: click in the Arrow Display cell (Drawing View menu) > select the section in which the arrows will be displayed > Apply. You can flip the direction using the Flip material removal side without re-orienting the view button > Close. You are done!!! for now.

To create a straight-line section (revolved) view: 2x-click the view you would like to section > in the Drawing View window > Categories: Section > 2D cross-section > click the plus (Add cross-section to view) button > Create new > in the XSEC CREATE menu > Planar > Single > Done > enter a section name (A, B, C) in pop-up window > OK. In the SETUP PLANE menu > Plane > pick a plane that will cut the view > apply > close. To add the section arrows click the Arrow Display cell in the Category: Sections > select the view > apply. An alternate way is: R-click the section view > Add arrows > LMB click the view you want to add arrows to.

The view showing the line-arrows sectioning profile can be displayed in Full, Half, Partial (isolate an area with a spline), and Broken (specify two points and direction to split the view), just check the Categories: Visible Area of the Drawing View window.

The view showing the actual hatched profile of the sectioned part can be displayed orthogonally [Full] or normal to the paper [Full(Unfold), Full(Align)], just check the Sectioned Area drop-down menu in the Categories: Sections of the Drawing View window.

To edit the hatching: 2x-click (LMB) the hatching > the MOD XHATCH menu appears: make your modifications > click Done or Quit.

To add or remove a sheet from the drawing: Layout [Document] > New sheet. Alternatively you can also R-click the current sheet tab and select Add new or Delete.

To enter Dimensions and Annotations: Annotate tab [Annotations] > Dimension > hold the Ctrl button and click the edges you want > MMB click to place dimension.

Retrieve Dimensions and Annotations from the 3D model: Annotate tab [Annotations] > Show Model Annotations > LMB click the view you want > select the dimensions/annotations you want to keep > apply > cancel. To change the properties of a dimension 2x-click on it and you can change some properties.

To change a dimension from one view to another: RMB-click the dimension, holding the RMB for about a second, then release > select Move item to view from the menu > click the new view.

To place a radius dimension: Annotate tab [Annotations] > Dimension > LMB-click ONCE on a curve > MMB to place the RADIUS dimension. Note: R-click to access pop-up menu and modify arrow positioning.

To place a diameter dimension: Annotate tab [Annotations] > Dimension > LMB-click TWICE on a curve > MMB to place the DIAMETER dimension.

To place a Hole Center Line: Annotate tab [Annotations] > Model Datum Axis > in the axis window enter a name, then > Define > chose the file name you want to work on > among the many choices pick Thru Cyl or Two Planes > pick the wall of the hole shaft > the reference line appears! > OK. This action should also place a corresponding center line in the other views.

To place a drawing note: Annotate tab [Annotations] > Note > LMB-click to place the note > type the text > check mark > in the NOTE TYPE window click Done/Return.

To place a surface finish note in the drawing file go to Annotate Tab > surface finish > in the dialog box browse for the Symbol Name and click OK.

To create a Bill of Materials in creo 4.0 drawing: Table [table] tab > table > Insert table. In the Insert Table window set the parameters as needed (column/row size, insertion point) and click OK. LMB select insertion point > Highlight a particular cell and hold the RMB and pick Height and Width from the pop-up menu > edit the parameters as needed.

To enter the heading on each column simply 2x-click the cell: In the Note Properties window Text tab type your text, in the Text Style enter appropriate justification and click OK.

In order for the table to expand and include all the information of all the parts contained in an assembly drawing we must set up the last row as a repeat row: Table [table] tab > Repeat region > select Add in the TBL REGIONS menu > LMB click on the top-left corner of the first cell to the left > MMB and check there is a small circle there > LMB click the bottom-left corner of that same cell, check for the circle > LMB click the top-right corner of the far right cell > MMB, check for marking circle > LMB bottom-right corner of the far right cell completing a quadrilateral region in that row > Done.

2x-click in the repeat region cell to add smart text. This text display the properties of the components in the assembly: to display ITEM number enter rpt.index, to display MATERIAL enter asm.mbr.ptc_material.PTC_MATERIAL_NAME, for the PART NUMBER: asm.mbr.name, the QTY cell: rpt.qty.

Display user-defined parameters in the BOM table: in the Part file define a parameter: Tools Tab > Model Intent > Parameters > click the Plus-sign Button to add a new parameter. Enter a Name, Type and Value, then click OK. Next in the Drawing File go to Table Tab > Data > Switch Symbols. In the Report Symbol window select asm.mbr.User Defined then you'll be promted to Enter Symbol Text, type the name of the parameter defined in the Part file, click check mark.

Stop the BOM table from creating duplicate entries: Table [table] tab > Repeat region > select Attributes in the TBL REGIONS menu > click the repeat region > select No duplicates > Done/return > Done. Now the table should display quantities in the corresponding column and identical parts should not repeat. Now to populate the drawing with corresponding balloons: Table [Balloons] > Create Balloons-All > select the populated region in the BOM table.

Enabling the ability for Tolerance Display: in the Drawing file go to File > Prepare > Drawing Properties. In the Drawing Properties window, next to Detail Options click change In the Options list window find tol_display click on it and change the value from no to yes. Click the Add/Change button > Apply > Close. Next, click on a dimension > in the Dimension Tab > Tolerance > pick your choice from Nominal, Basic, Limit, Plus/Minus, & Symmetric.