Introduction to Synchronous Modeling

Transcription

1 #SEU15 Introduction to Synchronous Modeling Craig Ruchti Global Technical Business Development Applications Engineer Realize innovation.

2 Introduction to Synchronous Technology Agenda Introduction Synchronous Technology what is it? Getting started Let us give you a hand The 7 biggest uses for Synchronous Let s see this in action! Page 2

3 Introduction: Craig Ruchti Craig Ruchti Solid Edge Global Technical Business Development Applications Engineer Craig Ruchti is a member of the Solid Edge Global Technical Business Development team (GTBD). This group creates Solid Edge demonstrations, produces and delivers technical Solid Edge update training and supports Solid Edge pre-sales activities globally. Craig is a graduate of the University of South Florida with a degree in Mechanical Engineering. Prior to working with the GTBD team, he worked designing rehabilitation engineering prototypes for various special projects and testing/altering existing designs to increase use and marketability. Page 3

4 Synchronous Technology: What is it? Synchronous Technology is a concept that allows users to work with 3D geometry and control their models without having to deal with underlying sketches. Once a piece of 3D geometry has been created, synchronous technology uses automatic design intent recognition tools to allow changes to be made in a predictable fashion, based on most frequent use cases. If at any time users wish to change the existing/recognized design intent, it s as easy as a single click or press of a hot key and the desired results are shown! Just think about the design potential with such freedom and power!! Page 4

5 Getting Started: Let us give you a hand! Synchronous Technology is different from Ordered/history based modeling. Need to make an edit? Just grab a face and begin to move using the arrow or steering wheel provided! Solid Edge interrogates the model during each edit and recognizes design intent that is worked in This is displayed for the user in an interactive dialog that allows it to be suppressed or turned on for each move Still having some trouble? Just click on the movie icon or the help button for a simple walk through! Page 5

6 The 7 biggest uses for Synchronous Synchronous Technology has incredible power and capability, but when is the best time to utilize it? 3D Detail Reuse Already created something similar in a previous design? Synchronous technology allows you to reuse that data in your new model! Design Intent Recognition Don t know who created this or how, but changes need to be made? Don t worry about underlying sketch design intent, what you see is what Solid Edge sees, as well as maintains! Editing Imported 3D data Importing foreign data such as a parasolid or STEP file? Get full control over your design with synchronous technology whether it was created in Solid Edge or not! One Shot Multi-Part Editing You ve seen the logic, now marvel at the power! Synchronous technology allows multiple faces on several different parts to be moved in a single action! Page 6

7 The 7 biggest uses for Synchronous - Continued Precise Direct Modeling Direct modelers have a bad wrap for not being precise. This isn t the case with synchronous technology. Complete control is offered through geometric relationships and dimensions, like you re used to in ordered! Rapid Initial Design Not 100% sure how the completed design will look? Synchronous is a great way to conceptualize by allowing you to get geometry on screen fast without worrying about having to start from scratch if you mess up! Unexpected Design Changes What happens when that geometry you got on screen fast needs to change? One of the key benefits to synchronous is being able to change design geometry and intent on the fly, without having to worry about those underlying sketches and order in which features were created! Page 7

8 Let s start by seeing an example of how solid edge automatically detects and maintains your design intent! For this example, we re going to run through a simple workflow using the ordered environment first, and then take a look at how synchronous handles the same situations Page 8

9 We need to make a few quick changes on this slide cylinder body Our first move we need to make is to Increase our overall height of the body to 31mm Select the body, and edit profile Page 9

10 Change the 29mm dimension to 31mm Accept and close the sketch Right click or click Finish Notice the planar view of the part: Page 10

11 We need to fix the cut on the side of the slide Select the cut feature and edit the profile Design intent wasn t built properly to accommodate for this change, so we ll need to fix this problem to keep the cut centered on the part Fence select the connect sketch relationship on the bottom of the sketch and delete it Once deleted, use the connect relationship to connect the top sketch line Do the same for the bottom Note: do not connect the end points to a keypoint Page 11

12 Now that we ve got the sketch centered, close the sketch environment Our next task is to thicken the stock between the cylinder and the bottom cut of the body We need 4mm of clearance, so let s use our smart dimension tool to determine how much material is there now On the home tab, select smart dimension on the dimension area Toggle the tangent dimension option Page 12

13 First, select the bottom radius (top of the cut) with a single click While still in the same command sequence, select the inside cylinder edge for the second selection Click to place the diminsion Note: This dimensions is simply informative. Ordered models cannot have PMI dimensions driving 3D geometry (dimensions only drive sketches) Page 13

14 Select the cut and edit the profile We need a total of 4mm clearance, currently we have 2.5mm We need to add 1.5mm to the 12.5 radius of the cut Page 14

15 Close the sketch back to the top level Right click or click Finish Notice the cylinder is now pushing up into the positioning holes Page 15

16 Obviously this wasn t our intent for this change luckily Solid Edge has some great Undo capability as well! Let s try it one more time select the cut and edit the profile The 1.7mm dimension is locked which keeps the cut moving upwards rather than downwards Unlock the 1.7mm dimension and place a locked dimension between the bottom edge and the midpoint of the radius Page 16

17 Now change the value of the radius to the 14mm we did before Close the sketch and check the part now Page 17

18 For our final change we have been having some blow through issues with some counterbore holes that carry the air for the pneumatics We need to move the top hole up 1mm, and the bottom hole down 1mm To get a better look at what we re working with, we re going to use a cutting plane to see inside the part On the View tab, select Set Planes from the Clip location Page 18

19 For the first step, we need to select a face for a reference plane to be coincident to Select the edge seen here After selection, ensure dynamic clipping is turned on in the properties Now drag the plane out to the outside of the part Page 19

20 Click to start the dynamic clip As you move the cursor to the left, the cutaway view of the internals of the part begin to show Move the cursor until our two counterbores are centered on the clipping plane Page 20

21 Right click to finish and accept clipping plane Zoom in and you can see where the issues are with wall thickness Turn off the clipping plane to work Select the bottom cylinder and edit the definition Page 21

22 Click on the 8mm dimension and change to 7mm Right click to accept Click on the upper cylinder and edit definition Notice that this feature was created differently than the first counterbore Page 22 Right click to end the edit

23 Rotate the model so you can see the cut on the inside of the large hole Edit definition of this hole Add 1mm to the dimension, making it 19mm Right click to accept Page 23

24 Turn back on dynamic clipping plane to make sure clearance is good All looks well, except that back hole is no longer centered with the first counterbore we moved We need to work in our desired design intent Page 24

25 Select the back hole and edit the profile Notice it s dimensioned to the bottom, rather than staying in line with the feed bore Select the 8mm dimension and delete it Select the horizontal/vertical option Connect the centerpoint of the cut to the centerpoint of the hole we wish to align it to Page 25

26 Click to close the sketch and go back to the part Turn off clipping planes Now let s see how synchronous could change our design process Page 26

27 Close the part, and DO NOT SAVE Page 27

28 Reopen Slide Cylinder Body.par Select the bottom feature on the pathfinder and right click Select move to synchronous Page 28

29 Now let s make the same moves as we did in ordered to compare Rather than having to edit underlying sketches, we can simply use the bodies Our first move is to change the overall height to 31mm Use the smart dimension tool, and select the two edges Page 29

30 Use symmetric input and enter 31 Press TAB (to stay in the command but not commit the change fully) Notice that design intent is automatically updated for both sides with symmetry and coplanar Click to uncheck to see how they update Accept dimension change with all design intent as defaulted (symmetric and coplanar turned on) Page 30

31 Our next move is to increase the amount of clearance between the cylinder and bottom cut Select the smart dimension command Click on the tangent option Select the bottom radius first, and the cylinder second Click to place Page 31

32 We don t have to worry about mathematics now, simply click the direction of the dimension change (we remember we want to push the cut downwards) Enter 4 for a value and once again, press TAB Notice the concentric and symmetric design intent is being maintained Accept the change as default Page 32

33 In just two quick dimensions we ve finished our first two changes! Our final change is going to be creating more clearance between the two counterbore holes So that we can see exactly what s going on, we re going to utilize a great tool called a synchronous live section On the home tab, click on Live Section under section For the planar reference, click the side of the slide cylinder with the cutout on it Page 33

34 While the live section is still highlighted and steering wheel showing, click the arrow perpendicular to the section and start moving it into the part As you move the live section through the part, ensure that centerpoint is the active snap points Snap the live section to the hole in the counterbore Page 34

35 Notice that live section gives you a view of all features that it s cutting! We want to keep an eye on that back hole, so we re going to place one more on the back face using the same technique Snap it in place of the back counterbore Page 35

36 The great part of live sections is they not only represent the features that lie on them, but the sketches can be controlled to change the geometry as well! Let s turn off the design body so that all we see are the sketches! Right click in the design area (the open white space) and click Hide All > Design Body Page 36

37 Let s also hide our PMI by unchecking it in the pathfinder Go to a planar view of the sketch that contains the counterbores we need to move Zoom in tight on the area where we ll be working Page 37

38 Since we need a symmetric change (1mm up, 1mm down) we re going to use another smart dimension First, select the top edge of the bottom counterbore Next, change the keypoint locate filter to Silhouette Select the silhouette point on the bottom of the upper counterbore Page 38

39 Drag the dimension outwards so that you can get the distance between the two edges Note: you need to be zoomed in close for this to work easily since the distance is so small! Zoom out with your scroll wheel as you move to place the dimension Page 39

40 Once placed, we re going to do a symmetric dimension Enter value to 2mm Press TAB to show the change but not accept it fully Page 40

41 Notice once again on the back hole, that design intent is picked up and those holes stay in line with one another! Click on and off aligned holes to see the model update Click to accept change with defaults Page 41

42 Now that everything is in order, let s turn on our design body to ensure the changes we wanted are the changes we got! Right click, Show All > Design Body Uncheck live sections in the pathfinder Page 42

43 CONGRATULATIONS! It s easy to see how sync can make changing workflows and designs a breeze without tripping over somebody else s design intent! Page 43

44 How about a little 3D detail reuse? Start by opening C:\\***\3D Detail Reuse\10mm Hose Custom Fittings Page 44

45 Next, on the Home tab, click on Coincident Plane command under planes Select the XZ plane on the base coordinate system to create a plane coincident to it Click to place While the plane is still highlighted, select the arrow from the steering wheel normal to the plane and click to move As the plane moves, key in 40 to move it 40mm Page 45

46 Next, on the Home tab, click on Hole in the Solids area Once in the Hole command, click on options In options, you want to set your standard to ANSI Metric and your hole size to 4 Click OK For the extent, ensure Through Next is selected Page 46

47 Mouse over the plane you created and when the plane highlights, press F3 or click the lock icon Now press Ctrl+H to get the model into a planar view Once in a planar view, position your cursor over the base coordinate system and place your first hole directly on the origin Once your first hole has been placed, mouse over the outside edge until the hole highlights, and press the C key This will measure off of your first hole and allow you to dimension subsequent holes directly off of that Key in 20 and go directly vertical to the original hole using the snap/dotted line Page 47

48 Repeat the exact same steps, except downward 20mm Page 48

49 The next portion of this is actually bringing in the connector geometry that we ve created in another part Open 15x10mm Reducer.par from the same area Page 49

50 Once we have the reducer open, we need to select all of the geometry we want to bring across Use the 3D view cube in the bottom right corner to put the part in a planar view of the front plane Fence select all of the smaller diameter geometry on the left Once all of that is selected, rotate the model slightly so you can pick up the inside cylinder of the same set of faces Page 50

51 Since our steering wheel is the handle in which we re going to hold all of this geometry, we need to place it properly so that we can control the reducer from a good point Click the origin of the steering wheel and ensure center point is an option for your snap points Now we want to snap that steering wheel in position on the base of the selected geometry as shown below: Page 51

52 Once placed, if your arrow normal to the torus is facing towards the middle of the part, we re going to have to flip it so that it comes in with the correct orientation Hold down the shift key and select the ball at the end of the arrow Holding the shift key allows the steering wheel to rotate around the highlighted arrow Key in 180 and press enter The correct orientation looks like this: Page 52

53 Now that we have our geometry selected and steering wheel oriented properly, we simply can copy and paste, just like in Microsoft office products! Click on the copy option on the home tab, or press Ctrl+C to copy Shift+Tab to go to our other part Ctrl+V will paste our geometry in place! Note: You should still be locked to the same plane, but if not, simply mouse over the plane and press F3 Page 53

54 Click anywhere on screen to place the geometry IMPORTANT!!! Do not deselect the geometry because we want to keep the steering wheel in place! Next, Select the small plane on the steering wheel to snap it to the Middle hole Your model should look like this: Page 54

55 In addition to being able to copy and paste, we might want to create a feature and place it in a library to use over and over This is simply done by clicking on the Feature Library side bar to expand it Now navigate to the same folder where the other parts are located, right click and click Paste Once pasted, name it 10mm hose connector_feature Page 55

56 Now all you have to do is drag and drop the feature and it will come in correctly every time! Let s do that drag and drop the feature onto our part and place it on the top hole using the same steps as before Drag and drop Page 56

57 Prior to de-selecting the connector, we want to change the top and bottom ones up a bit Hold Shift and click the arrow normal to the torus Pull out 15mm Page 57

58 Now that we have our steering wheel offset, click on the same arrow as the direction of the offset (normal to torus) and snap it to the centerpoint of our hole again As you re making this move, notice that you re getting a orange color stating that the move isn t working Page 58

59 Not to worry! This is just live rules telling you that there is some design intent it s picking up that you might not want to change! The faces on the new feature are located EXACTLY in line with the faces on the first placed feature. This is considered coplanar! Notice on the design intent bar, it s telling us that coplanar has been detected. So if we want to move just one of these, we can simply turn off coplanar and voila! Page 59

60 Now that we have our second set of faces in place, we need to move this down to the bottom hole We can do this how we ve done the previous two Copy/paste Feature library But here, we re just going to use a copy/move to accomplish this task! Hold the Ctrl key down Just like in Microsoft office products, Ctrl is a command for copy Select the bottom arrow Snap new face set to the bottom hole Page 60

61 Everybody should be looking at this: Page 61

62 Now that we have all of our feature sets in the proper position, we need to attach them to the model Check this out!!! Hold Ctrl and select all three of the face sets at the bottom of the pathfinder Right click > Attach Page 62

63 Whoa!!!! Solid Edge can look at the ends of the surfaces of features and if it can resolve when extending them, it will automatically do so and make them part of the body they re extending into! Page 63

64 Now that we see how our piece is coming together, I don t think the tubes are going to be able to fit the connectors the way they re positioned The great part about synchronous is that we can change pretty much whatever we want, whenever we want all we have to work with is what we see on screen Lets make an angular offset on the top and bottom prongs Fence select all of the geometry on the upper connector Now do the exact same for the bottom Page 64

65 We want to rotate these two connectors 15 degrees around our cylindrical base Select the origin of the steering wheel and snap it to the top of the cylindrical base Click to place it Click on the torus to rotate Notice once again we re getting the operation unsuccessful orange feedback Page 65

66 Whenever this happens, it simply means that Solid Edge s design intent has picked up that something might be changed that the user might not want So lets go to our design intent box We can see that aligned holes is being picked up This means that it s saying Hey, this middle hole is in the same vertical location as the two outside ones. Are you sure you want to move just these two? Click on Aligned Holes or press A on your keyboard Page 66

67 Rotate the connectors out 20 degrees and click to place Page 67

68 Continuing on not only can our copy/paste capability add material to a model, it can also subtract, as well as bring in additional intelligence! Expand Design Bodies in the pathfinder Turn on Fuel Flow Sensor and Double click to make it the active body Page 68

69 We re going to bring in a feature from our feature library On the feature library side pane, double click on the flow sensor folder Select Feature_Fuel Flow Sensor Housing.par Click and drag in Page 69

70 Next we need to orient the feature to a plane Mouse over the top face of the fuel flow sensor body and press F3 to orient Page 70

71 Click to place the feature anywhere on the top face BUT DO NOT DESELECT THE ASSOCIATED FACES Click on the arrow shown below and snap to the centerpoint keypoint on the block below Page 71

72 Now select the arrow to center the feature in the middle of the face Make sure midpoint is selected as your keypoint locate option Snap the feature into place using the midpoint Page 72

73 Once centered, right click on the face set at the bottom of the pathfinder Select Attach Page 73

74 The best part about these intelligent feature is that you have full control over them after the fact! Select the PMI dimension on the slot Change the value, using symmetric input to 6mm Page 74

75 Additionally, let s take a look at those holes! Select one of the holes Click on where it says M2 and change to M2.3 Notice that not just one hole, but all of the holes associated to the feature update! Also notice that the holes are standard driven Page 75

76 3D Detail Reuse! Congratulations! Page 76

77 Contact Craig Ruchti Applications Engineer Global Technical Business Development 675 Discovery Dr NW #100 Huntsville, AL Phone: +01 (256) Mobile: +01 (256) Realize innovation. Page 77