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Objective 1: Roll Geometry Into a Cylinder

Objective 1: Roll Geometry Into a Cylinder. The objective of this tutorial is to demonstrate techniques which can be used to roll a flat sheet into a cylinder (tight spiral). Parameters will be used to capture critical variables required to generate a cylinder using a Spiral of Archimedes.

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Objective 1: Roll Geometry Into a Cylinder

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  1. Objective 1: Roll Geometry Into a Cylinder The objective of this tutorial is to demonstrate techniques which can be used to roll a flat sheet into a cylinder (tight spiral). Parameters will be used to capture critical variables required to generate a cylinder using a Spiral of Archimedes. Detailed View ~80” Beginning Geometry .01” Thk Flat Sheet w/ repeating tabs along the top/bottom edge

  2. Preparation: Configuration Options In order to work with the very detailed features in our example model, it will be necessary to set several configuration options before we begin. First, we must set the model accuracy finer than the default accuracy range allows. To accomplish this, reset the lower accuracy boundary by selectingToolsOptions and setting the accuracy_lower_bound option to .00001 as shown below. 4

  3. Setting the Accuracy Set the accuracy of the model to .00001 by selectingFilePropertiesAccuracyChange Enter .00001 and selectRegenerate Modelas shown below. Close the Properties dialog box to proceed.

  4. Setting the Model Display Properties To insure the tight curves in this tutorial are displayed smoothly on screen, set the Edge Quality to Very High by selecting ViewDisplay SettingsModel Display From the Edge/Line tab, set the Edge Quality as shown.

  5. Beginning Geometry This tutorial assumes pre-existing geometry with irregular features will be rolled into a cylinder. Starting from scratch, there are other, less cumbersome techniques for rolling/unrolling a cylinder. However, these techniques usually begin with a spiral curve or cylinder and end with flat geometry. This procedure begins with flat geometry and ends with a spiral cylinder. Flat Geometry Rolled Geometry

  6. Spiral/Coil Parameter Definitions coil_outer_dia coil_inner_dia coil_gap_thk coil_sheet_thk These 4 parameters will be used to create the spiral curve equation in subsequent steps.

  7. Spiral Curve Reference Requirements Curves created from an equation require a single coordinate system as a reference. For this tutorial, the spiral will be created in the X-Y plane (the “Top” plane) and centered on the Z axis. The CSYS below has been named for convenience. Placement of this coordinate system feature is important. Place it along one edge of the solid geometry in the location you want the spiral to begin. See Next Slide for details. Solid Geometry Removed for Clarity

  8. Important Considerations for Spiral CSYS The coordinate system for the spiral should fall along a solid geometry edge. Notice that the spiral below falls on the end of the flat geometry with the Z axis aligned to the vertical edge. Note the location of the CSYS along the rear edge of the solid geometry +Z Axis Aligned to this Edge This slide intended only to illustrate CSYS placement. Spiral curves will be created on the next slides! Spiral Curve Isometric View Reference Only Spiral Curve Top View Reference Only

  9. Overview: Steps for Rolling Solid Geometry Step 1: Create parameters to define spiral (req’d in Step 3) Step 2: Create a coordinate system as the starting reference for a spiral curve. Step 3: Create a Curve From Equation to define the spiral. Step 4: Extrude a surface from the spiral curve which will be used as a wrapping reference. Step 5: Wrap a sketched copy of the solid geometry around the reference surface from previous step. Step 6: Trim away unused portions of the reference surface. Step 7: Thicken the reference surface to create the solid. Although the remainder of this tutorial documents the steps required to create the specific geometry shown in the examples, you should apply the lessons learned to your own designs. Experiment with the sample models to gain additional insights into the techniques presented. For example, change the orientation of the reference coordinate system in Step 1 or alter the equations shown in Step 2 to see the effect of these modifications. Detailed Instructions For Each Step Follow on Next Slides

  10. Step 1: Create Parameters to Define Spiral From the top Pro/ENGINEER menu, select ToolsParameters. Enter the four new parameters and the values shown below. See Slide #7 to review the parameter definitions. These parameter values will be changed later. We’re using them as an initial start point.

  11. Step 2: Create a Reference CSYS Create a coordinate system as the starting reference for a spiral curve. Locate the coordinate system keeping in mind the requirements and considerations on Slides 8 & 9. +Z Axis Isometric View CSYS Placement Detail Top View CSYS Placement Detail

  12. Step 3: Create a Spiral Curve From Equation To create a CurveFrom Equation, from the top menu selectInsertModel DatumCurveor use the Datum Curve icon circled below. Select From Equation and Done from the menu to proceed. When the Curve dialog box opens, select the coordinate system created in the previous step. Choose Cylindrical as the Csys Type. The relation editor will automatically open (see next slide).

  13. Step 3: Creating a Curve (Cont) The Relation Editor will automatically open with some default comments. From the editor window, selectFileOpen and load the file “spiral_relation.txt” included with the tutorial files. The modified file appears below. • Relation Notes • All lines beginning with “/*” are comments • For a cylindrical equation (used in this example), you must define each of the following three variables: • r – radius • theta – angle of rotation (polar) • z – depth • When Z is equal to zero, the curve will remain flat and coplanar to the reference coordinate system

  14. Step 3: Creating a Curve (Cont) From the editor window, selectFileSave to save the relations. Select FileExitto exit the editor and return to the Curve dialog box. Select OK to complete the curve definition. A spiral curve will appear centered on the reference coordinate system as shown below. Top View Spiral Curve Detail

  15. Step 4: Extrude a Surface from the Curve Start the Extrude tool (InsertExtrude). Select the “Top” datum plane as the sketch plane. Once in Sketch Mode, select SketchUse Edge and select the curve. Select the entire curve with the Use Edge function. This will copy the curve as the sketch for the Extrude feature Select “Top” as sketch plane Top View Spiral Curve Detail

  16. Step 4: Extrude a Surface (Cont) Complete the sketch by selecting to return to the Extrude Tool dashboard. Set the dashboard as shown below turning on the Surface option and setting the depth symmetrical to 5.00 inches. When done, complete the feature by selecting Set the Surface option here Use Symmetric depth Set depth value to 5.00 Extrude Dashboard Options Extrude Preview

  17. Introducing the Wrap Tool The Wrap Tool provides the ability realistically wrap a sketch around any surface. For our demonstration model, we’re using the extruded surface from Step 4 as our reference surface. One limitation of the Wrap Tool is that it cannot be used directly on solid geometry. Therefore, we will generate a sketch which mimics the solid geometry outline and use this copy within the Wrap feature. The procedure for this technique begins with Step 5 on the next slide.

  18. Step 5: Wrap a Sketch Around Surface Start the Wrap Tool by selectingEditWrap from the top Pro/E menu. Select the References sub-tab from the dashboard as shown below. Select the spiral surface created in Step 4 as the Destination reference. Select Define to define the sketch. Wrap Target will be changed to Sketcher CSYS later Define sketch Select spiral surface as Destination reference Wrap Tool Dashboard

  19. Step 5: Wrap a Sketch (Cont) Orient the sketch such that you have a full view of the solid geometry. For our demonstration model, the orientation is shown below. SelectSketchUse Edge (or use the icon) and pick the Loop radio button as shown. Select the front surface of the solid geometry. The entire outline of the part should be copied. Selecting “Loop” insures the sketch will always update to include the entire solid geometry outline Partial View of Solid Geometry after Loop Selection

  20. Step 5: Wrap a Sketch (Cont) Next, create a SketchedCoordinate System by selectingSketchCoordinate Systemfrom the top menu (or by using the icon shown here from the side flyout menu). Snap the new sketched coordinate system to the edge of your sketch at the center datum plane. Long sketched edge (orange line - hard to see) Sketched CSYS should snap to the midpoint of the edge. In this case, the CSYS will fall on the center datum plane. Drag the new sketched CSYS toward the midpoint of the long edge

  21. Step 5: Wrap a Sketch (Cont) Complete the sketch by selecting to return to the Wrap Tool dashboard. Change the Wrap Target to Sketcher CSYS. Note that this option will remain greyed out unless a coordinate system was created in the sketch as shown on the previous slide. Direction Control Change Wrap Target to Sketcher CSYS Wrap Tool Dashboard When done, complete the feature by selecting If the feature fails, flip the direction using the Direction Control.

  22. Step 5: Wrap a Sketch (Cont) The final geometry for Step 5 is shown below. Surface Geometry Hidden to Show Curves Curves Shown Wrapped Around Reference Surface

  23. Step 6: Trim Portions of Reference Surface A surface trim allows us to cut away portions of a surface using a curve as the cutting tool. To use this tool, select extruded surface created in Step 4. With the surface highlighted, selectEditTrim from the top menu. Select the References sub-tab. The pre-selected surface should already appear as the Trimmed Quilt reference. Select Details next to the Trimming Object reference to continue. By pre-selecting the surface before starting the Trim Tool, the reference will appear here automatically Click here to select a curve to use as a cutting tool Trim Tool Dashboard

  24. Step 6: Trim Reference Surface (Cont) From the Chain dialog box, select the radio button for Rule-based as shown. Also select Partial Loop as the rule type. In the next slide, we’ll select the top loop of curves as a cutting tool for the surface trim. Top Portion of Wrapped Curves Shown (Surface Hidden for Clarity) Our intent in the next slide is to select only the wrapped curves along the top edge of the surface and use them as a cutting tool. Chain Dialog Box Spiral Surface with Wrapped Curves

  25. Step 6: Trim Reference Surface (Cont) Looking only at the top portion of the spiral surface, select the inside and outside end curves as boundaries for the partial loop. The two end curves are shown in Red below. The system should select the chain of curves in between (as shown highlighted in orange below). See next two slides for additional views & tips. Outside End Curve Shown Selected in Red Inside End Curve Shown Selected in RedChain Loop Shown Selected in Orange

  26. Step 6: Trim Reference Surface (Cont) In some circumstances, the system will highlight the chain of edges in the wrong direction. If this happens, select the Flip command shown below. Sometimes you’ll have to explicitly pick inside the Extent Reference box (shown below) before you can pick the second end curve. Select the box here (in Green) to reactivate the curve reference collector if you find you cannot pick the second end curve Click here to flip the direction of the chain

  27. Step 6: Trim Reference Surface (Cont) The top views below are intended as additional visual aids to assist in selecting the partial curve chain. The system should automatically select the Partial Loop chain in Orange. Outside End Curve Shown Selected in Red Inside End Curve Shown Selected in RedChain Loop Shown Selected in Orange

  28. Step 6: Trim Reference Surface (Cont) Once the chain has been selected, close the Chain dialog box. Pay attention to the yellow directional arrow. The arrow points to the portion of the surface to keep after the trim. If necessary, select the Flip command to change the cut direction. When done, select to complete the feature. Flip Command Trim Curve & Surface Selected Yellow Arrow Shows Direction to Keep Trim Tool Dashboard

  29. Step 6: Trim Reference Surface (Cont) Repeat Step 6 for the lower loop of curves. The final trimmed surface (top & bottom) appears below. Detailed View of Trimmed Surface Final Trimmed Surface

  30. Step 7: Thicken the Trimmed Surface Highlight the trimmed surface from Step 6 and selectEditThicken from the top menu. Enter the desired depth and direction to thicken. Complete the command to finish the procedure. Top View Isometric of Final Wrapped Geometry Top View (Dark Background) of Final Wrapped Geometry

  31. Objective 1: Review Notes • To further automate the model, use relations to drive the thickness of the solid flat geometry and the thicken feature in Step 7 from the coil_sheet_thk parameter (defined in Step 1) • Be aware that the extruded surface in Step 4 should extend beyond the limits of the flat geometry. If the extruded surface doesn’t extend beyond the flat geometry, the wrapped curve will fail. • Selecting the top/bottom partial loops can be simplified by using Intent Chains but this is beyond the scope of this document • Inheritance, Copy Geometry, Flexible Features, and Family Tables all provide methods for displaying the model in the flat or rolled state.

  32. Objective 1: Review Notes (Cont) • At times during the creation of this tutorial, the relations loaded in Step 3 failed to save properly. If this occurs, open the spiral_relations.txt file and copy/paste the text into the Relations Editor (rather than attempting to import the file). This resolves the problem. • The Curve From Equation may need to be slightly tweaked to account for material thickness. (For example, one material thickness may need to be removed from the outer diameter to keep it within the desired boundaries). • If geometry fails to regenerate at any step, be sure to check the model accuracy, references, direction of features, and critical dimensions. • Failure to keep the sketcher coordinate system directly on the edge of your sketch in Step 5 can cause the feature to fail.

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