Techniques for Troubleshooting Sketches &

Transcription

1 Techniques for Troubleshooting Sketches &

2 Written by Tim Brotherhood These materials are 2001 PTC Conditions of use Copying and use of these materials is authorized only in the schools of teachers who attend official training and have received a legal site license. All other use is prohibited unless written permission is obtained from the copyright holder. Acknowledgements John Hutchinson - The College of New Jersey Troubleshooting Page 82

3 Contents Problems with sketches...84 Redundant sketches...84 Deleting a feature...84 Editing the sketch...85 Un suppress feature...85 Self intersecting - revolve...84 Rigid sketches...87 Moving a sketch...87 Renaming Sketches, workplanes, features...88 Synchronizing browser to sketch...88 Rename a sketch...89 Synchronizing browser to a feature...89 Rename a feature...89 Problems creating solids...89 Self intersecting - Sweep...90 Mirror the path...90 Relocate the profile sketch...92 Create two sweeps...92 Create a third sweep...93 Creating A Mechanism Fixing Components...93 Nothing moves - no freedom of movement...95 Too much movement - not enough constraints...95 Over constrained...95 Synchronizing the browser...96 Identifying a constraint...96 Deleting a constraint...97 Add new constraint...97 Quiz - Correcting faults/design...98 Troubleshooting Page 83

4 Intermediate Pro/DESKTOP Techniques This tutorial is intended to develop your skills in finding and solving problems with sketches. By working through these exercises, you will become skilled in a number of intermediate and advanced Pro/DESKTOP techniques. Problems with sketches Redundant sketches Often, inexperienced users try to create a feature such as extrude when the sketch is invalid. The feature fails, an error is reported and the user chooses the suppress option. The unsuccessful feature is created but inactive. Normally the sketch is then edited to make it valid before the feature is un-suppressed and the model updated. Unfortunately it is not uncommon for people to make two or three further attempts to create the feature storing up duplicate suppressed features. These will need to be deleted to clean up the design prior to fixing the sketch and removing suppress from the remaining feature and updating the design. Open the file called Suppress fault1.des. Change the Units to millimeters. (Pull-down menu: Tools > Options > Units). Change the Browser to show Features. You will notice there are three failed extrusions. This is indicated by the red X symbols. You will need to find out which one has the correct extrusion distance of 30mm, deleting the others. Right click over extrusion 1. Select Properties from the floating menu. Note the extrusion distance and close the window. Repeat the previous steps to check the other two extrusions. An extrusion distance of 30mm is required so extrusion 2 is the one we want to keep. Deleting a feature Right click over Extrusion 1. Select Delete from the floating menu. Repeat these steps for Extrusion 3. Troubleshooting Page 84

5 Editing the sketch The profile would appear to be made up of four arcs and yet there are eight small nodes around the perimeter suggesting eight arcs. Zoom in on one of the small pairs of nodes in the profile sketch. Using, the Delete line segment tool, you can pre-highlight an overlap in the lines. Delete one of the small overlap lines. Repeat these steps with the three other dual nodes. Open the line menu and select Toggle sketch filled. Notice how the sketch looks now: there is a single dark red node at each place lines meet around the perimeter. This is the characteristic of a valid sketch. The sketch should be shaded to show it is now a valid profile. Un suppress feature Right click over the extrusion. Click on the suppress option in the floating menu to un-suppress the feature. Click on, the Update design button. The extrusion should occur successfully. Troubleshooting Page 85

6 Self intersecting - revolve This error can occur when the profile overlaps the axis. Valid sketches for Revolve Invalid sketches for Revolve It should be a simple task to move the axis line away from the profile. Open the file Self intersect - revolve1.des. Notice which workplane and sketch are currently active (base workplane and Axis sketch are bold in the workplane browser). Troubleshooting Page 86

7 Double click on one of the lines in the profile of the wheel. The sketch containing that line becomes the active sketch in the workplane browser. In this case the Wheel profile sketch. Rigid sketches The Wheel profile sketch has been made Rigid. This allows you to move the entire sketch in one go without it changing shape. The rigid option can only be applied to a complete sketch. Hint: Making a sketch rigid is different to fixing lines. Individual lines can be fixed selectively to prevent them from moving in the sketch. Moving a sketch Use the, tool to select the bottom line in the wheel profile. Move the mouse cursor over the selected line. When the pre-highlight indicates the left hand end of the line, click and drag the sketch into the position shown below. Release the mouse button when the co-ordinates read 3,0. Snap to Grid (3, 0) Note: Picking the sketch up by pointing to the left hand end of the line allows you to locate the new position accurately to leave an axle hole of 6mm diameter. How else could you control the distance between the axis line and the profile sketch? Troubleshooting Page 87

8 Revolve the profile to show it will do so successfully. Have a go with a similar problem in the file named Self intersect test.des. Hint: You should also make sure the axis line is on different sketch to the profile. Renaming Sketches, workplanes, features If workplanes, sketches and features are not given sensible names the task of finding and correcting faults is made very difficult. As models become complex or several students need help at the same time, teachers might consider refusing to assist until students assign meaningful names to sketches and features! Encouraging good practice from the beginning may avoid the need to resort to such drastic measures. It is relatively straightforward to rename workplanes, sketches, and features. The file Die finished.des has most things named sensibly. Exceptions are sketch 6 and extrusions 8 and 11. Before you can assign more sensible names to these you will need to find out where the sketches are in the model. Synchronizing browser to sketch Open the file Die finished.des. Make sure the browser is set to Workplanes. Click on the + next to Lft frnt. Right click over the sketch name Sketch 6. Click on Select lines in the floating menu. Three circles highlight red. A sensible name for this sketch would be Three. Troubleshooting Page 88

9 Rename a sketch Right click over the name sketch 6. Select Properties from the floating menu. Change the name to Three. Click on. The new sketch name is more relevant. Synchronizing browser to a feature Make sure the browser is set to Features. Right click over Extrusion 11. Click on Select Edges in the floating menu. Four circles highlight red. A sensible name for this sketch would be Four. Rename a feature Right click on the extrusion named Extrusion 11. Select Rename from the floating menu. Change the name to Four. Click on. Repeat the previous steps to identify where Extrusion 8 is on the model and rename it appropriately. What would be a sensible name for this workplane? Do not save the model so that it is ready for the next person. Problems creating solids At the stage where solids are created, a number of things can go wrong. Perhaps the most common fault is a self-intersecting solid. This was explained previously using the example of a revolved shape, as the solution involved moving lines in a sketch. You may also get this error when creating a sweep and the solution is slightly different. Troubleshooting Page 89

10 Self intersecting - Sweep Open the file called Self intersect - sweep1.des Half of the heart shape has been created in 3D using the sweep feature. Notice how the profile sketch (a circle) has been located at the intersection of the two arcs making up the path. This is one of the few places where the two workplanes containing the path and profile are perpendicular. It should be a simple task to mirror the path along the center axis and update the model. Mirror the path Make sure the path sketch is active in the browser. Shift-click both path lines making up the right half of the heart. Open the Line pull-down menu and select mirror Click on the Axes tab. Click to select the construction line along the central axis of the heart. This will be used as the mirror. The lines being created by the mirror tool will be previewed in the model. Click on. Troubleshooting Page 90

11 An error message will appear reporting an Internal Error has occurred. This is one of only a few unhelpful messages Pro/DESKTOP produces. Nevertheless it offers no clues how to solve the problem. Analyzing the path and profile may suggest why there is a problem and point to solutions we can try. The path in the crevice at the top of the heart doubles back on itself. This might have produced an error describing an attempt to create a self-intersecting solid. Maybe this is the problem? One solution would be to remove the cusp in the path at this point. Make sure the path sketch is active. Select, the arc or fillet tool. Drag an arc to radius the join at the center of the heart. Update the extrusion and the result should be successful. We may have achieved a solution but the shape of the heart has been compromised. Is there another solution that will retain the purity of the original shape? Two possible solutions spring to mind. Troubleshooting Page 91

12 1. Relocate the profile sketch to the center of the path at the cusp. 2. Create the two halves of the heart with separate sweep features. Relocate the profile sketch Change to the profile sketch. View Onto Workplane. Select the circle. Drag it to the origin. Try Updating the design. Oops! The same error message appears so this is not a solution. Create two sweeps Leave the profile sketch at the center. Double click on one of the path arcs to activate the path sketch Select the two arcs forming the left half of the path. From the Edit menu select Cut. Create a new sketch on the base workplane called left path. Paste the arcs onto this sketch. Update the design with the, button. The original half heart should be the result. Troubleshooting Page 92

13 Create a new Sweep feature using the original profile and the new left path. The result is almost exactly the desired outcome. Notice the join at the bottom of the heart is not very neat. How could we solve this problem? Create a third sweep Create another new sketch on the base workplane called bottom half path. Cut and paste the two curves making up the bottom half of the path onto the new workplane. Create another profile sketch on the Frontal workplane called Lower half profile. Hint: The profile circle must lie along, and perpendicular to, the path line. Carry out another Sweep for the lower half. Mission accomplished! Close the design without saving. Creating A Mechanism Fixing Components In the next section you will create a moveable mechanism and gain an understanding of how Pro/DESKTOP can be used to analyze and design mechanical systems. For this section change Units to inches. Create a bar link about 8 long, 1.25 wide and 0.25 thick with a 0.25 diameter hole in the middle and one at each end concentric with the rounded ends. Save the file as Link.des. Start a New Design file and save it as Link Assembly.des. In this new file use the Pull-down menu Assembly > Add Component and select Link. Use the Select Parts tool and click on the Link object and release. The cursor arrow should now have a small box attached to it. This indicates that Troubleshooting Page 93

14 you can now click and drag the object around the screen. Move the Link a bit to the left. You are doing this because the next Link you bring in to the file will come in over top of the first and you might not see it. Bring another Link into the Design. Assembly the two Links by using Center Axes command so that the center hole on one link is aligned with the center hole on the other. Mate the two facing surfaces. Next we will Fix one of the links in place. This will keep everything from moving around on the screen and help us see the mechanical movement. Select the lower link and right-click. Choose Fix Component from the floating menu (you could also use Assembly > Fix Component from the pull-down menu). Bring in a third and forth Link and assemble them to the first two as seen below. Click on one of the the last Link and release. Then click and drag that Link and see the way in which the system moves. Although there is no surface collision detection to prevent solid objects from passing through each other, the ability to create mechanical systems is a very powerful tool for design. When first trying to move an assembly using kinematics everything moves on screen. It is customary to fix one component around which all other movement takes place. Troubleshooting Page 94

15 Nothing moves - no freedom of movement Open the file called Link assembly2.des. Here the model has been assembled with an extra cross brace. This triangulates the end of the mechanism preventing any movement. Try selecting and dragging a component to 'exercise' the mechanism. Too much movement - not enough constraints Open the file called Link assembly3.des. Select a component and try dragging to move the mechanism. Before movement After movement The mechnism quickly becomes deranged because there are insufficient assembly constraints to control the components. Try applying more constraints to make the assembly work correctly. Close the design without saving. Over constrained This usually happens when a constraint is being added that is obviously impossible. A good example is a parallelogram frame with a diagonal brace. Open the file called Link assembly4.des. Try to constrain the loose strut across the horizontal diagonal. The length is obviously too short and so the final constraint is impossible as it would 'over constrain the assembly'. Troubleshooting Page 95

16 Synchronizing the browser This technique is useful to identify individual components in the browser list. Open the file toy assembly.des in the Toy folder Activate, the Select part tool. Click on a wheel to select it. Right click on the wheel. Select Synchronize browser from the floating menu. The browser changes to Components and one of the Plain wheels will be selected. Click on the + sign next to the highlighted wheel. A list of constraints that apply to the wheel will appear. This method can be used to identify any component in the browser. Identifying a constraint Right click over the Center constraint. Click on Select defining geometry from the floating menu. The surfaces making up the Center constraint will be highlighted in red. Hint: You may need to view in wireframe (F9) to see it effectively. Troubleshooting Page 96

17 Deleting a constraint Right click over the same constraint and this time select Delete. The wheel is no longer constrained concentrically on the axle. Activate, the Part select tool, highlight and drag the wheel away from the engine. Add new constraint Practice re-assembling the wheel to the axle. Close the assembly without saving the file. NOTES The skills you have learned in this section broaden the opportunities for using Pro/DESKTOP to design products. There will be times when you will want to design products that you can prototype or model. Other opportunities where products could not possibly be manufactured should not be dismissed. Worthwhile learning experiences can result from design situations where the context is so far removed from personal experience that design issues become the main focus of the activity. Troubleshooting Page 97

18 Quiz - Correcting faults/design 1. How can you tell a feature has a fault? 2. How would you delete a faulty feature? 3. There can be very small gaps or overlaps between lines in a sketch. How would you locate these? 4. Which tool in Pro/DESKTOP can you use to check whether a sketch is valid? 5. The Revolve Profile feature relies on two sketches, an axis and a profile. If each sketch is valid why might the feature fail to work? 6. Give one advantage of making a sketch rigid. 7. How would you go about renaming a sketch? 8. What method would you use to find out which lines are on a specific sketch? 9. How do you create a mirror of lines in a sketch? 10. How do you stop a complete assembly moving on screen? 11. Try to identify if a component in the browser is straightforward. How would you do this? 12. How can an assembly constraint be deleted? 13. Why is the design specification very important? 14. At what stage(s) does a designer refer back to the specification? Troubleshooting Page 98