Mold Design & Manufacturing Process

Transcription

1 CATIA Demonstration Script Mold Design & Manufacturing Process PDF by The demonstration Image Medium size 400X300 Version 5 Release 13 February 2004 C513_demMold_Script_DesignManufacturing Page 1

2 Setting up CATIA Environment Setting up CATIA Environment Erase previous Settings If your CATSettings folder has not been created in V5R13, you must first physically delete it and restart CATIA. The file is located in folder C:\Documents and Settings\user_name\Application Data\DassaultSystemes Tool/Options Click button Resets parameters values to default ones and select option for all the tabpages This is necessary only if the previous erase has not been done Tools/Options/General : General : set Data Save : No automatic backup Display/Performances : set 3D Accuracy : Fixed = 0.01 Page 2

3 Setting up CATIA Environment Setting up CATIA Environment Tools/Options/General : Parameters and Measures/Knowledge : activate Parameter Tree View : With value & With formula Tools/Options/Infrastructure : Product Structure/Tree Customization : activate Specification Tree Order : Parameters, Relations, Constraints Part Infrastructure/Display : activate Display In Specification Tree : Constraints, Parameters, Relations Page 3

4 Setting up CATIA Environment Setting up CATIA Environment Tools/Options/Mechanical Design : Assembly Design/General : set Update : Automatic Sketcher : deactivate Grid : Snap to point Tools/Options/NC Manufacturing : Photo/Video : set Simulation at : Part operation level Page 4

5 Demo Steps 1 2 Step 1 Data Check and Repair Step 2 Applying local Deformation Step Core & Cavity Separation Step 4 Parting Surface Definition 5 Step 5 Mold Tool Design Step 6 Mold Tool Drawings Step and 3-Axis Manufacturing 7 6 Page 5

6 Step 1 : Data Check and Repair Check Input data : Face Validity Enter workbench Healing Assistant Open Design Part Open file \Step1- InputDataCheck&Repair\Begin\ CarHandle.CATPart Part has previously been read from IGES file It is made up of about 210 independent surfaces Check intrinsic validity of all surfaces Multi-select all surfaces Click icon Face Checker Keep Self-Intersection default value : mm Click button Apply One Face is diagnosed with Self- Intersection Page 6

7 Step 1 : Data Check and Repair Repair Input data : Face Validity Separate invalid surfaces : Click button Transfer In dialog box Transfer, activate Reframe On in contextual menu of the line Site.1 Corresponding face is highlighted in the 3D viewer Click Move button to move Site.1 from list Anomalies Detected to list Anomalies Selected Page 7

8 Step 1 : Data Check and Repair Repair Input data : Face Validity Repair invalid surfaces : Activate option Automatic Repair Click button Close Surface.92 has been identified as invalid and a new repaired Surface has automatically been created and put in a dedicated separate Geometrical Set The initial invalid surface is automatically put in NoShow in a dedicated separate Geometrical Set In dialog box Face Checker, click OK to validate the operation Hide all elements except the faulty surface and zoom : The extremities are very sharp : the boundary of the face is probably not clean enough and some of its edges are crisscrossing. Delete Geometrical Set containing original invalid surface Surface.92 Put back the remaining elements in Show Page 8

9 Step 1 : Data Check and Repair Check Input Data : Face Connections Analyze quality of connection between all surfaces : Multi-select all visible surfaces Click icon Surface Connection Checker : Default value for Connection distance = mm Default value for Search distance = Regular = 0.1 mm These values give the range (min/max) of analysis Below the min value, two edges are considered as identical. It corresponds to the target value of the Join to be performed later to concatenate these independent surfaces. Between min and max values, two edges are candidates for merging via Local Join or Local Healing operations Beyond the max value, elements correspond to functional holes and should not be Joined or are defect faces that should undergo repair before being Joined. Page 9

10 Step 1 : Data Check and Repair Check Input Data : Face Connections Change value of Connection distance to 0.01 mm : this is a realistic target value for the future Join of all Surfaces Click Apply The dialog box displays analysis results for all criteria : Duplicate, Embedded, Multiple Connection, All results are computed simultaneously : by selecting one criterion in the list, you switch the graphical highlight in the 3D viewer to the current active criterion (e.g. Duplicate displayed in purple, Multiple Connection in dark blue, etc. Page 10

11 Step 1 : Data Check and Repair Check Input Data: Duplicate Faces Focus first on duplicate surfaces : Make sure that the current selected option in the dialog box is Duplicate : 1 duplicate face has been detected Separate duplicate surfaces : Click button Transfer In dialog box Transfer, click Move button to move Site.1 from list Anomalies Detected to list Anomalies Selected Click button Close A new Geometrical Set has automatically been created to group together the two surfaces detected as identical In dialog box Surface Connection Checker, click button OK to validate the operation Delete redundant surfaces : Delete Geometrical Set called Surplus to eliminate one of the identical surfaces Page 11

12 Step 1 : Data Check and Repair Check Input Data : Embedded Faces Focus now on embedded surfaces : Multi-select all visible surfaces Click icon Surface Connection Checker Keep values : Search distance = Regular = 0.1 mm and Connection distance = 0.01 mm Click Apply to perform analysis for all criteria Select criterion Embedded One location has been detected Separate embedded surfaces : Click button Transfer In dialog box Transfer, click Move button to move Site.1 from list Anomalies Detected to list Anomalies Selected Click button Close A new Geometrical Set has been created In dialog box Surface Connection Checker, click button OK to validate the operation Page 12

13 Step 1 : Data Check and Repair Repair Input Data : Embedded Faces Delete unnecessary surfaces : Put the new Geometrical Set in Show mode Hide Surface.130 : you can see that Surface.129 is embedded in Surface.130 Delete Surface.129 Page 13

14 Step 1 : Data Check and Repair Check Input Data : Overlaps Focus now on overlapping surfaces : Multi-select all visible surfaces Click icon Surface Connection Checker Keep previous values : Search distance = Regular = 0.1 mm and Connection distance = 0.01 mm Click Apply to perform the analysis for all criteria Select criterion Overlap 4 locations have been detected Note that solving the duplicate and embedded cases first has helped reduce the number of overlaps, which was equal to 6 after the first Surface Connection Checker analysis. Page 14

15 Step 1 : Data Check and Repair Repair Input Data : Overlaps Separate overlapping surfaces : Click button Transfer In dialog box Transfer, click Move All button to move Site.1 from list Anomalies Detected to list Anomalies Selected Click button Close A new Geometrical Set has automatically been created to group together the surfaces causing the problem Click button Transfer Page 15

16 Step 1 : Data Check and Repair Repair Input Data : Overlaps In dialog box Transfer, click Move All button to move Site.1 from list Anomalies Detected to list Anomalies Selected Click button Close A new Geometrical Set has automatically been created to group together the surfaces causing the problem Prepare rework of the surfaces : Show the newly created Geometrical Set Change the colour of its surfaces (e.g. light blue) to recognize them more easily Page 16

17 Step 1 : Data Check and Repair Repair Input Data : Overlaps First rework action : delete unnecessary surface : Delete Surface.147 which is superimposed on Surface.257 Second rework action : replace surface causing overlap : Focus on connection between Surface.78 and Surface.84 Zoom in to check the overlap visually Delete Surface.84 Create a new Geometrical Set and make it current Page 17

18 Step 1 : Data Check and Repair Repair Input Data : Overlaps Click icon Create datum Click icon Fill Select the edges of the neighbour surfaces to create a new Surface as shown Click OK to validate creation A warning message informs you that there is a 0.01 mm gap between the element No further action is required now : this gap will be handled later via the Merging distance of the Join operation Page 18

19 Step 1 : Data Check and Repair Repair Input Data : Overlaps Third rework action : trim extremity of surface causing overlap : Focus on connection between Surface.78 and Surface.62 Zoom in to check the overlap visually You can see that the sharp extremity of Surface.78 is deeply overlapping with Surface.62 There are no neighbour edges which can be reused directly to replace this sharp Surface by a new one, so we are going to trim its extremity Click icon Create datum Click icon Boundary and select Surface.78 Click OK to validate creation of boundary Curve Hide Geometrical Set.1 for better visualization Page 19

20 Step 1 : Data Check and Repair Repair Input Data : Overlaps Click icon Create datum Click icon Projection Select Projected = boundary Curve Select Support = Surface.62 Click OK to validate operation Hide original boundary Curve Click icon Create datum Click icon Line and select User type = Point-Point Pick successively the two vertices of the projection Curve Select Support = Surface.62 Click OK to validate creation Click icon Create datum Click icon Projection Select Projected = line Curve Select Support = Surface.78 Click OK to validate operation Page 20

21 Step 1 : Data Check and Repair Repair Input Data : Overlaps Click icon Create datum Click icon Split Select Element to cut = Surface.78 Select Cutting element = projected Curve Make sure the appropriate side of Surface.78 is pre-visualized Click OK to validate operation Delete the wireframe construction elements previously created Delete Surface.78 Page 21

22 Step 1 : Data Check and Repair Repair Input Data Create Join with all Surfaces Show Geometrical Set.1 Create a new Geometric Set Multi-select all visible surfaces Click icon Join Deselect option Check Connexity Set merging distance = 0.01 mm Click OK to validate Compute remaining free edges Select Join Click icon Boundary Click OK Click No in dialog box Multi-result management in order to keep all subelements The Boundary is created Page 22

23 Step 1 : Data Check and Repair Repair Input Data Repair remaining free edges with Local Join+Healing Select new Boundary Click icon Local Join Default option is Join You can see that the system has computed the minimum Merging Distance for the join : 0.05 mm Set Join Merging Distance = 0.05 mm Select option Automatic Join/Heal Click Apply There are no visible free edges (green display) Click OK to validate Page 23

24 Step 1 : Data Check and Repair Repair Input Data Check Join closure Select Local Join Click icon Boundary A message informs that the Join is closed Click Cancel to cancel Boundary creation Close without Save End of Step 1. Result data is : \Step1-InputDataCheck&Repair\End\ CarHandle.CATPart Page 24

25 Step 2 : Applying local Deformation Local Part Deformation Dedicated analysis or previous experience show that the inner hole is subject to deformation when hot plastic injection is done. To offset this effect, the opposite deformation can be applied to the original shape to ensure that the final result is really a round hole. This deformation will be applied thanks to function Shape Morphing (workbench Generative Shape Optimizer is necessary). Applying the deformation will be applied in a quick and convenient way thanks to Powercopy capability. Page 25

26 Step 2 : Applying local Deformation Applying local Deformation Open the Design Part : Open file \Step2- LocalDeformation\Begin\CarHandle.CATPart Make sure that Generative Shape Design is the current active workbench Select PowerCopy of Part Deformation Template Click Insert / Instantiate From Document Select file \Step2- LocalDeformation\Begin\PowerCopyLocalDe formation.catpart Dialog box Insert Object is displayed The Design Part is going to be modified to change the shape of the inner hole from round to ellipsoidal in order to compensate for the deformation during the injection operation. Page 26

27 Step 2 : Applying local Deformation Applying local Deformation Select the Part to be deformed Pick the Local Join feature This corresponds to expected PowerCopy input named PartSkin Select the original round hole curve Pick prepared red curve called OriginalCurve-Circle This corresponds to expected PowerCopy input named InitialCurve Select the target ellipse curve Pick prepared green curve called TargetCurve-Ellipse This corresponds to expected PowerCopy input named DeformedCurve Page 27

28 Step 2 : Applying local Deformation Applying local Deformation Define two fixed curves to control the deformation of the Part Pick the edge at the extremity of the Part as shown This corresponds to expected PowerCopy input named FixedCurve-1 Pick the edge on the upper side of the Part as shown This corresponds to expected PowerCopy input named FixedCurve-2 Define a limit curve to control the propagation of the deformation Pick the edge as shown This corresponds to expected PowerCopy input named CurveForNormalPlane This edge will be used by the PowerCopy to compute a normal plane through it. The intersection of this plane and the Part will be the limit curve to propagate the deformation Make sure the green arrow is oriented as shown in order to define the correct orientation for propagating the deformation. Page 28

29 Step 2 : Applying local Deformation Applying local Deformation Pick the vertex as shown This corresponds to expected PowerCopy input named PointForNormalPlane This point will be used by the PowerCopy to compute the normal plane, then the limit curve mentioned before. Create the deformation Click button Preview to check the computed result Click OK to validate the creation of the Shape Morphing feature Hide Local Join to better visualize the final result Close without Save End of Step 2. Result data is : \Step2-LocalDeformation\End\ CarHandle.CATPart Page 29

30 Step 3 : Core & Cavity Separation Create Molded Part Import Part to mold Create new empty Product and make it active (highlighted in orange) Enter workbench Core & Cavity Design Click icon Import model Select Reference = \Step3- CoreCavitySeparation\Begin\CarHandle.CAT Part Select Body = DeformationElements Surface Shape Morphing.1 is automatically selected Select Axis System = Local axis system Select shrinkage : Scaling Ratio = 1.01 Click OK to validate Reframe on the Part A solid element (ClosedSurface) has been created and the corresponding scaling value has automatically been applied Page 30

31 Step 3 : Core & Cavity Separation Define Main Pulling Direction Define Mold areas Click icon Define pulling direction Drag and drop compass origin (red square point) onto the bottom of the inner hole of the part Click anywhere on the part A coloured display shows the mold areas of the part : Core in Red, Cavity in Green, Other (to be reworked) in blue, and No Draft (vertical faces, according to value of Draft angle) in pink Click button Reverse if necessary This is to ensure that Z+ axis of the pulling direction is oriented towards the outer side of the Part and that Core side (red) corresponds to the inner side of the Part Activate option Locked This will prevent any erroneous displacement during further operations Page 31

32 Step 3 : Core & Cavity Separation Define Main Pulling Direction Refine mold areas : Facets to ignore Zoom in onto one of the blue faces located among the Core side Select option Visualization = Facet display to check the defects You can see that these faces are not quite moldable because of insufficient quality of design. However, the defects are not too big, so we will reassign these faces to Core side. A similar analysis could be done for other blue faces Select option Visualization = Face display Activate option Facets to ignore Keep default maximum ratio value (15 %) You can see that many blue faces have been automatically transferred to Core side or Cavity side Page 32

33 Step 3 : Core & Cavity Separation Define Main Pulling Direction Refine mold areas : Explode mode Activate option Visualization = Explode Set the translation value to 50mm Core side (red faces) and Cavity side (green faces) are moved apart accordingly, thus enabling to see more clearly which remaining blue faces could be redistributed to Core or Cavity areas. Refine mold areas : Local Transfer to Core Activate option Local Transfer Keep default destination = Core Select propagation type = No propagation Click the two blue faces as shown Page 33

34 Step 3 : Core & Cavity Separation Define Main Pulling Direction Refine mold areas : Local Transfer to Cavity Select default destination = Cavity Keep propagation type = No propagation Click the blue faces as shown Click OK to validate the creation of the Mold areas. Further rework has still to be done Four Geometrical Sets have automatically been created : Core, Cavity, Other, NoDraft An Axis System has automatically been created (Main Pulling Direction.1) Page 34

35 Step 3 : Core & Cavity Separation Define Slider area Define Slider area Click icon Defines slider lifter direction Drag and drop the compass onto the inner face of the undercut area Note that the corresponding face has switched from pink to yellow, which is the typical colour of a Slider/lifter area Activate option Locked Activate option Local Transfer Keep default destination = Slider/Lifter Select propagation type = Point continuity Pick successively pink, blue, green and red faces of the undercut area Click OK to validate A new Geometrical Set has automatically been created : Slider/Lifter.1 An Axis System has automatically been created (Main Pulling Direction.1) Page 35

36 Step 3 : Core & Cavity Separation Refine Mold areas : Reflect Line Compute Reflect Line Create a new Geometrical Set Zoom onto the remaining blue area : this region of the Part has to be reworked because the Reflect Line corresponding to the Main Pulling Direction is crossing it. Hide Mold areas Other, Core, Cavity Show Part Body The Reflect Line will be computed on the corresponding region of thepart itself. It is not computed on the Mold area, since this Mold area will then be split by the Reflect line (it would cause a logical loop). Click icon Reflect Line Select Support = Scaling.1 Select Direction : Z axis of Main Pulling Direction Select Angle = 90 deg Click OK to validate Page 36

37 Step 3 : Core & Cavity Separation Refine Mold areas : Reflect Line Restrict Reflect Line Click Yes in dialog box Multi-Result Management The Reflect Line is made up of several discontinuous pieces : we will keep only the relevant piece Pick one face or edge near the desired piece of the Reflect Line Click OK to validate Page 37

38 Step 3 : Core & Cavity Separation Refine Mold areas : Split by Reflect Line Split Mold area Other Hide Part Body Show Mold areas Other, Core, Cavity Click icon Split mold area Select propagation type = Point continuity Pick one blue face Select Cutting Element : Near.1 Keep default destination = Core Click Apply Click button Switch Destination if necessary to ensure the appropriate side of the Split goes to the Core area Click OK to validate Page 38

39 Step 3 : Core & Cavity Separation Refine Mold areas : Transfer Faces Transfer remaining blue faces to Cavity area Click icon Transfer an element Select Propagation type = Point continuity Select Destination = Cavity Pick one blue face Click OK to validate Final check Click icon Explode View Set Explode Value = 50 mm Click Cancel to close Exploded View Close without Save End of Step 3. Result data is : \Step3-CoreCavitySeparation\End\ Product1.CATProduct Page 39

40 Step 4 : Parting Surface Creation Define External Parting Surface Open Molded Part Open file \Step4- PartingSurfaceCreation\Begin\MoldedPart.CATPart Enter workbench Core & Cavity Design Aggregate Mold areas Click icon Aggregate Mold Area Select Geometrical Set Core Activate option Create a join datum Validate Core side is now a single connex surface without free edges Repeat previous operations on Cavity side. Page 40

41 Step 4 : Parting Surface Creation Define External Parting Surface Start creating Parting Surface elements Click icon Parting surface Deactivate option Join Parting Surface Start with Cavity side Pick the Cavity area as Reference Support Create first Extrude Successively pick the two vertices as shown The piece of boundary between the two vertices is highlighted in green Pick the line of the prepared sketch as shown An Extrude surface is created The sketch is located in the plane orthogonal to the Main Pulling Direction Page 41

42 Step 4 : Parting Surface Creation Define External Parting Surface Create second Extrude Successively pick the two vertices as shown Pick the line of the prepared sketch as shown An Extrude surface is created Create third Extrude Successively pick the two vertices as shown Pick the line of the prepared sketch as shown An Extrude surface is created Page 42

43 Step 4 : Parting Surface Creation Define External Parting Surface Create fourth Extrude Successively pick the two vertices as shown Pick the side of the prepared sketch as shown An Extrude surface is created The sketch is located in the plane orthogonal to the Slider Pulling Direction Create first Loft Click icon Multi-section Surface in the dialog box Successively pick the two vertices as shown Successively pick the two sections as shown (reverse orientation of first section with red arrow) A Multi-section surface is created Page 43

44 Step 4 : Parting Surface Creation Define External Parting Surface Create second Loft Successively pick the two vertices as shown Successively pick the two sections as shown (reverse orientation of first section with red arrow) A Multi-section surface is created This Surface will be reworked later to add tangency constraint in order to get a smoother shape Continue with Core side In the dialog box, click icon Extrude In the dialog box, select field Reference In the 3D viewer, pick the Core area as Reference Support Page 44

45 Step 4 : Parting Surface Creation Define External Parting Surface Create Extrude Successively pick the two vertices as shown The piece of boundary between the two vertices is highlighted in green Pick the line of the prepared sketch as shown An Extrude surface is created The sketch is located in the plane orthogonal to the Main Pulling Direction Validate creation of all surfaces Click OK in dialog box Parting Surface Creation You can see that the corresponding surfaces have been created as Extrude and Multi-sections Surface features Page 45

46 Step 4 : Parting Surface Creation Define External Parting Surface Rework a previous surface to add tangency Double-click the Multi-section surface as shown In the dialog box, select line of Section no.1 In the 3D viewer, pick the neighbour Extrude Surface as shown Tangency constraint is added Click OK to validate the modification Page 46

47 Step 4 : Parting Surface Creation Define External Parting Surface Create last surfaces : Sweep Click icon Sweep Select as Profile the edge of the Extrude as shown Select as Guide Curve the edge of the Extrude as shown Click OK to validate Create another Sweep surface as shown The definition of the outer Parting Surface is now complete Page 47

48 Step 4 : Parting Surface Creation Define Splitting Surfaces Start defining splitting surfaces Create a new Geometrical Set and call it SplittingSurfaces Fill functional Hole Click icon Fill Select the edges of the inner hole Click OK to validate Join external Parting Surface elements common to Cavity side and Core side Click icon Join Multi-select adequate surfaces created previously (in light blue on the picture) Set Merging distance = 0.01 mm Click OK to validate Page 48

49 Step 4 : Parting Surface Creation Define Splitting Surfaces Create complete splitting surface for Cavity Side Click icon Join Multi-select adequate surfaces : Cavity area, Fill surface, previous Join, specific Extrude (in dark blue on the picture) Set Merging distance = 0.01 mm Click OK to validate Rename new Join as CavitySurface Change its colour to dark green Create complete splitting surface for Core Side Proceed similarly to create a Join for the Core side Specific Extrude is in light pink on the picture Rename new Join as CoreSurface Change its colour to dark pink Page 49

50 Step 4 : Parting Surface Creation Define Splitting Surfaces Create complete splitting surface for the Slider Click icon Join Multi-select adequate surfaces : Slider area, specific Extrudes (in dark blue and light pink on the picture) Set Merging distance = 0.01 mm Click OK to validate Rename new Join as SliderSurface Change its colour to bright yellow Close without Save End of Step 4. Result data is : \Step4-PartingSurfaceCreation\End\ MoldedPart.CATPart Page 50

51 Step 5 : Mold Tool Design Reuse existing User Mold Base Template Enter workbench Assembly Design Create a new empty Product Select the Mold Base Template Click icon Catalog Browser In the dialog box, click icon Browse another catalog In dialog box File selection, doubleclick \Step5- MoldToolDesign\Begin\UserMoldBases.c atalog There are two categories of templates in the catalog Double-click item named Type- TwoPrints Double-click item named SmallSize Page 51

52 Step 5 : Mold Tool Design Reuse existing User Mold Base Template Create the Mold Base Double-click item named TwoPrintsWithInserts Dialog box Insert Object is displayed, showing the Product Template Click OK in dialog box Insert Object A message informs you that the documents of the Template have been instantiated : the Mold Base Product, but also the prepared associated Drawing Click OK to acknowledge the message Click Close in dialog box Catalog Borowser The Mold Base Product is created Note that it already includes various components : Leader Pins, Bushings, etc. Page 52

53 Step 5 : Mold Tool Design Reuse existing User Mold Base Template Close the Drawing Select Drawing document in the list of open documents Do not update it and save it with a meaningful name in a folder of your choice. We will focus on the drawing in a next step A message informs you that the corresponding Product is modified but not saved. Click Yes in message dialog box. Another message lists the details of unsaved Product and Parts files. Click Yes in message dialog box. Page 53

54 Step 5 : Mold Tool Design Insert Molded Part in Mold Assembly Enter workbench Mold Tooling Design Insert Molded Part in the Mold Base Select top Product It is now highlighted in orange Select Insert / Existing Component Select file \Step5- MoldToolDesign\Begin\MoldedPart.CATP art Click OK to validate The Molded Part is now inserted in the Assembly, but its position has to be adjusted Page 54

55 Step 5 : Mold Tool Design Insert Molded Part in Mold Assembly Adjust the position of the Molded Part Hide Injection Side Click icon Snap First, select Axis System.3 (pale blue) in the Molded Part Then select Axis System.2 (dotted line yellow) in the Core Plate The Molded Part is now correctly positioned on the first Insert instance of Core side Adjust the size of both Inserts Activate icon Top View Select in the tree the first Insert instance In contextual menu, activate Insert object / Edit Insert Component Select tab Parameters Set Insert width W = 140 mm Click OK to validate update of both inserts Page 55

56 Step 5 : Mold Tool Design Split the two Inserts Split the Insert instances Double-click Part Insert_1_1.1 in the specification tree to make it active Make sure the active workbench is now Part Design Click icon Split In the Molded Part, select published surface named CoreSurface Check the preview to ensure the kept side is the one as shown Click OK in dialog box Split Definition Hide component Molded Part You can see that both Insert instances have been simultaneously split Page 56

57 Step 5 : Mold Tool Design Change Insert orientation Rotate second insert Double-click top Product Make sure the active workbench is now Mold Tooling Design Select in the tree the second Insert instance In contextual menu, activate Insert object / Edit Insert Component Select the rotation spinner (green halfcircle) In contextual menu, activate Edit angle Set Angle = 180 deg Click OK to validate in dialog box Edit Insert The second Insert is now positioned head-to-tail with the first one to allow for easier positioning of the Injection Gates and Runners Page 57

58 Step 5 : Mold Tool Design Create Ejectors Define Ejectors locations Double-click any of the pink sketch points The Sketcher is now active Zoom in onto one of the inserts Drag and drop the existing two points to relocate them approximately as shown Zoom in onto the second insert to check that the two other points of the sketch have automatically been adjusted This is because these points have been created symmetrical to the first ones Click icon Exit workbench Double-click top Product in the tree to switch back to workbench Mold Tooling Design Page 58

59 Step 5 : Mold Tool Design Create Ejectors Select and position the Ejectors Click icon Add Ejector Click the Open file icon Select file \Step5- MoldToolDesign\Begin\Hasco\Ejector_Z 41_1.CATPart This standard Hasco Ejector has been customized to include a userdefined Knowledgeware Rule which will be described later Pick any of the four pink sketch points A preview of four instances of the Ejector is displayed Click button Reverse Direction to define upward orientation Page 59

60 Step 5 : Mold Tool Design Create Ejectors Define Ejector drillings In dialog box Define Ejector, check that field Drill From has automatically been set to EjectorPlateB (this is the plate containing the sketch) Select field To in order to make it current In the 3D viewer, pick the Insert Field To is automatically updated Click button Between From and To In the 3D viewer, pick successively CoreSupportPlate and CorePlate In dialog box Define All Components to Cross, click OK to validate the list Page 60

61 Step 5 : Mold Tool Design Create Ejectors Define Ejector dimensions In dialog box Define Ejector, select tab Parameters Pick any of the two Design Table icons In the Design Table dialog box, change the current configuration (D = 1mm, L = 200mm) to D = 1.5mm, L = 200mm Click OK to validate this selection Note that the fitting length of the Ejector is set to 10 mm (parameter Offset_Parting shown in the panel) In dialog box Define Ejector, click OK to validate the creation of the four Ejectors Page 61

62 Step 5 : Mold Tool Design Create Ejectors Split Ejectors In the specification tree, multi-select the two Ejectors located in the first Insert Activate in contextual menu : Selected objects / Split component Dialog box Split Definition is displayed CoreSurface is automatically displayed as default choice for splitting Click OK to validate Split operation Zoom in onto the two Ejectors to see the result Page 62

63 Step 5 : Mold Tool Design Create Ejectors Measure fitting length Zoom in onto the Ejector located on the thickest side of the Insert Click icon Measure Between Select the top edge of the split Ejector Select the bottom edge of its fitting tip (use arrow to select through the material) This is the edge resulting from the Remove of DrillHole in the Insert You can see that the fitting length = 10 mm, i.e. the value defined in Ejector s parameter Offset_Parting Click Cancel Page 63

64 Step 5 : Mold Tool Design Create Ejectors Show Knowledgeware Rule to adjust the fitting length In the specification tree, unfold node Relations of the Ejector Part Highlight Knowledgeware Rule named FittingLengthComputation Double-click it once to activate workbench Knowledge Advisor Double-click it again to open the Rule Editor dialog box and display the content of the Rule This Rule enables to adjust the fitting length of the ejector to value Offset_Parting whatever the location of the Ejector Click OK to close the Rule Editor dialog box Double-click the top Product in the tree to switch back to workbench Mold Tooling Design Page 64

65 Step 5 : Mold Tool Design Create Ejectors Change Ejector location Select again the same Ejector in the tree In contextual menu, activate Ejector object / Edit component Click icon Top View Use the green arrow spinners to drag the Ejector to the bottom of the pocket as shown Click OK to validate the new location Click icon Measure Between Select the top and bottom edges as done previously You can see that the clearance hole of the Ejector has been adjusted to keep the fitting tip length at 10 mm Page 65

66 Step 5 : Mold Tool Design Create Slider Mechanism Prepare Slider positioning Show Component Molded Part Hide Geometrical Set PartingBody Green positioning point predefined in MoldedPart is now visible Create dedicated sub-structure in the Mold Assembly In the tree, double-click Product Mold to make it active Select Insert / New Component Select Properties in the contextual menu of the new component Set Part Number = MovingElements Click OK to validate In the tree, double-click the new Component to make it active It is now highlighted in blue Page 66

67 Step 5 : Mold Tool Design Create Slider Mechanism Select Slider Assembly Click icon Add User Component Click the Open file icon Select file \Step5- MoldToolDesign\Begin\SliderAssembly\ DressedSlider.CATProduct Define Slider position Pick green positioning point predefined in MoldedPart A preview of the Slider Assembly is displayed Use the green arc spinner to define a 90-deg rotation The Slider assembly preview should now look as shown Page 67

68 Step 5 : Mold Tool Design Create Slider Mechanism Define Slider position Click icon Top View Set position U = -5 mm Click Tab key to refresh the preview Define the drillings Select field To Pick CorePlate in the 3D viewer The CorePlate will be drilled by the DrillHolde of elements Slider, Retainers, AnglePin The CorePlate will be drilled by the TapHole of elements CapScrews Create Slider Assembly Click OK to validate creation Check the drillings Hide component MovingElements to show the drillings in the Core Plate Show again MovingElements Page 68

69 Step 5 : Mold Tool Design Create Slider Mechanism Split Form part of the Slider Zoom in onto the form part of the Slider Select Component Slider in the Slider assembly user component In contextual menu, activate Slider object / Split component Show Geometrical Set named PartingBody in the MoldedPart In the tree, select surface named SliderSurface Click button Display direction to check it as shown on the picture Click OK to validate Split operation Page 69

70 Step 5 : Mold Tool Design Create Slider Mechanism Final check Hide PartingBody The form part of the Slider now fits the undercut area Close without Save End of Step 5. Result data is : \Step5-MoldToolDesign\End\ Product1.CATProduct Page 70

71 Step 6 : Mold Tool Drawings Start from Drawing Template Open Tool Product Open file \Step6- MoldToolDrawings\Begin\CarHandle- TwoInserts.CATProduct Close dialog box with warning message Open corresponding Drawing Open file \Step6- MoldToolDrawings\Begin\TwoPrintsWithIn serts.catdrawing The template is made up of 3 views : Front View of complete Mold from top, Section View of complete Mold lengthwise, Section View of complete Mold widthwise. The predefined title block template will have to be updated (names, etc.) Page 71

72 Step 6 : Mold Tool Drawings Create the Bill of Material Automatic numbering of the Parts Select the Product in the list of open documents Switch to workbench Assembly Design In the specification tree, double-click Product Mold It is now highlighted in orange Click icon Generate Numbering Keep default values (Mode = Integer) Click OK to validate numbering operation Create the Bill of Material Select Analyze / Bill Of Material Page 72

73 Step 6 : Mold Tool Drawings Create the Bill of Material Customize the Bill of Material Click button Define formats In section Properties for the Bill of Material, click button Hide all properties In section Properties for the Recapitulation, transfer successively properties Nomenclature, Material and Number by using button Show properties Click OK in dialog box Define formats Click OK in dialog box Bill of Material Note that property Number contains for each Part the value defined by operation Generate Numbering Page 73

74 Step 6 : Mold Tool Drawings Create the Bill of Material Insert the Generative BOM in the Drawing Select Window / Tile Horizontally Select the Drawing window Activate contextual menu of Sheet.1 and select Activate Sheet Select Insert / Generation / Bill of Material Select node Mold in the specification tree of the Product Pick in the Drawing Sheet the location where you want to insert the BOM Zoom in to check the content of the BOM Page 74

75 Step 6 : Mold Tool Drawings Complete the Drawing Update the Title Block Select Edit / Background Double-click the text frame of the drawing title and change initial value xxx to Car Handle Click OK in dialog box Text Editor Select Edit / Working Views Global change in the definition of Section View Select Section View B-B In its contextual menu, select Edit Properties Uncheck option Hidden Lines Click OK to validate The View is automatically updated Page 75

76 Step 6 : Mold Tool Drawings Complete the Drawing Change Section View Profile Double-click the profile defining Section B-B Click icon Replace Profile Create a new profile approximately as shown Click icon End Profile Edition The Section View is automatically updated Page 76

77 Step 6 : Mold Tool Drawings Complete the Drawing Local change in definition of Section View In contextual menu of Section View B-B, select Section View B-B Object / Overload properties Dialog box Characteristics is displayed Select the Slider The corresponding line is created in the Characteristics dialog box Click button Edit In dialog box Editor, deactivate option Cut in section views and activate option Represented with hidden lines Therefore the hidden lines of this component will be displayed. Click OK in the two dialog boxes The view is updated Page 77

78 Step 6 : Mold Tool Drawings Complete the Drawing Create Balloons Click icon Generate Balloons Arrange the position of some overlapping balloons Close without Save End of Step 6. Result data is : \Step6-MoldToolDrawings\End\ TwoPrintsWithInserts.CATDrawing Page 78

79 Step 7 : 2.5- & 3-Axis Manufacturing Start Manufacturing of one Insert Start from existing Machining Process Open file \Step7- Manufacturing\Begin\Template_3Xroughing.CATProcess Select Product to be machined In the PPR tree, double-click Part Operation In dialog box Part Operation, click icon Product or Part Select file \Step7- Manufacturing\Begin\Product_for_demo nstration.catproduct Page 79

80 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Select Part to be machined In dialog box Part Operation, click icon Design part for simulation Double-click the Insert in the 3D viewer Define rough stock In dialog box Part Operation, click icon Stock In PPR tree, double-click Part Body of the Part named STOCK This is the rough Pad defining the Insert, before the Insert is split with the form surfaces Page 80

81 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Define a safety plane In dialog box Part Operation, click icon Safety plane Select plane XY in the 3D viewer In the 3D viewer, activate contextual menu of the Safety plane Select Offset Set Thickness = 70 mm Click OK to validate Offset creation Click icon Left View Zoom in a little to check the position of the Safety plane Click OK in dialog box Part Operation to validate Part Operation Page 81

82 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Define areas to be machined Click icon Manufacturing View In dialog box Manufacturing View, activate in contextual menu : Manufacturing View object / Sort by Machinable Features Double-click item Part to be machined In dialog box Zone : Areas, click the sensitive area In the 3D viewer, first select the Insert (Part Body), then Filling Surfaces (Geometrical Set) Double-click in the background to get dialog box Zone : Areas back Click OK in dialog box Zone : Areas Page 82

83 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Define limiting contour In dialog box Manufacturing View, double-click item Limiting Contour Definition In dialog box Zone : Lines, click the sensitive edge area In toolbar Edge Selection, click icon Display option panel In dialog box Options, make sure that Link types = Line insert Pick successively the four corner edges of the Insert to get a result as shown In toolbar Edge Selection, click icon Close Contour with Line to close the contour Click OK in toolbar Edge Selection Click OK in dialog box Zone : Lines Click Close in dialog box Manufacturing View Use Save As to store CATProcess in another folder of your choice Page 83

84 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Define computation in batch mode Click icon Manage Batch Queue In dialog box NC Batch Management, click icon New job In dialog box Job definition, click icon In the PPR tree, select 3-Axis PROGRAM In dialog box Job definition, click OK to validate Page 84

85 Step 7 : 2.5- & 3-Axis Manufacturing Define Roughing Operations Start batch computation In dialog box NC Batch Management, click button Activate Click Yes in message panel to start execution of the batch queue Click OK in next message panel to acknowledge it In dialog box NC Batch Management, click OK to close it Next machining operations (semifinishing, finishing) can now be defined interactively while roughing operation is computed in batch Synchronization of these operations with the result of batch computation will be done later Page 85

86 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Define Slope area Click icon Machining/Slope Area Activate contextual menu of sensitive area named Part Activate Select zones In dialog box Zone Selection, select line Part to be machined Click right-arrow button to transfer it to list Selected Click OK to validate selection In dialog box Machining Area, activate option Slope Area Select tab Slope Area Select T3Ball-Nose D16 as Reference Tool Set Lower Angle = 47 deg Set Overlap = 1 mm Page 86

87 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Customize predefined Slope Area machining strategy Select tab Operations Activate field Insertion Level In the PPR tree, select operation Roughing.3 Select area Horizontal Select Assign = Sweeping Click OK to validate Two new operations have been automatically created in the PPR tree : ZLevel and Sweeping The resulting sequence should be as shown. In the last Tool Change operation, make sure that Zlevel appears before Sweeping Page 87

88 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Compute Tool paths In the PPR tree, multi-select operations ZLevel and Sweeping Click icon Tool Path Replay Both tool paths are successively computed and displayed Simulate Tool path In dialog box Sweeping.1, click icon Go to start of tool path Click icon Forward replay Simulation of the ZLevel operation begins Page 88

89 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Simulate Tool path After a few seconds, click icon Display complete tool path The simulation now runs until the end of the Sweeping operation Click OK in dialog box Sweeping to close it Page 89

90 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Load additional semi-finishing operations from existing catalog Click icon Open Catalog Click icon Browse another catalog Select file \Step7- Manufacturing\Begin\Machining_Process es.catalog Double-click chapter 3-AXIS OPERATIONS Double-click MachiningProcess.2 Locate new operations in the current process In the PPR tree, select last operation (Sweeping) Corresponding information is updated in dialog box Insert Object Page 90

91 Step 7 : 2.5- & 3-Axis Manufacturing Define Semi-finishing Operations Define geometry to apply loaded operations Click icon Manufacturing View Select Pencil Semi-Finishing Corresponding information is updated in dialog box Insert Object Click OK in dialog box Insert Object Click Close in dialog box Catalog Browser Click Close in dialog box Manufacturing View Check the PPR tree : two new operations have been inserted (Pencil.1 and Pencil.2) Compute tool paths Multi-select the two Pencil operations Click icon Tool Path Replay Both Tool Paths are now computed Click OK in dialog box Pencil.2 Page 91

92 Step 7 : 2.5- & 3-Axis Manufacturing Define Finishing Operations Define Rework operations Click icon Rework area In dialog box Rework Area, click button Load from Select Sweeping.1 in the PPR tree Sensitive area Part has turned green in dialog box Rework Area Click tab Other in dialog box Rework Area Set tolerance = 0.02 mm Select tab Operations Select field Insertion Level Select Pencil2 in the PPR tree Select Tool Reference = T5 Ball- Nose D4 Click OK to validate definition Check the PPR tree : two new operations have been inserted : Contour-driven.1 and ZLevel.2 Page 92

93 Step 7 : 2.5- & 3-Axis Manufacturing Define Finishing Operations Define Rework operations In the PPR tree, double-click operation Contour-driven.1 to edit it In dialog box Contour-driven, set Machining tolerance = 0.03 mm Click OK to validate Similarly, edit operation Zlevel.2 to also set Machining tolerance = 0.03 mm Compute Tool Path Multi-select operations Contourdriven.1 and ZLevel.2 Click icon Tool Path Replay Both Tool Paths are now computed Page 93

94 Step 7 : 2.5- & 3-Axis Manufacturing Define Finishing Operations Visualize computed Tool Path In dialog box ZLevel.2, click icon Go to start of tool path Click icon Forward replay Simulation of the Contour-driven operation begins After a few seconds, click OK in simulation dialog box to end the dynamic visualization Page 94

95 Step 7 : 2.5- & 3-Axis Manufacturing Synchronize Result of Batch Recall batch result Click icon Manage Batch Queue Select computed program in dialog box NC Batch Management Click icon Synchronize a computed job in dialog box NC Batch Management Click Yes in message panel to get the batch-computed tool path Status is set to Synchronized in the dialog box Click OK to validate The Roughing operations appear as Computed in the PPR tree Page 95

96 Step 7 : 2.5- & 3-Axis Manufacturing Check Results Check Roughing operations with video simulation Select operation Roughing.3 in the PPR tree Click icon Tool Path Replay Result appears instantly In dialog box Roughing.3, click icon Video from last saved result Click icon Forward replay Move the speed cursor far right to accelerate the simulation All three Roughing operations are successively displayed After a while, click OK to end dynamic visualization Page 96

97 Step 7 : 2.5- & 3-Axis Manufacturing Check Results Check final result with video simulation Select operation ZLevel.2 in the PPR tree Click icon Tool Path Replay In dialog box ZLevel.2, click icon Mixed Photo/Video Click icon Forward replay The toolpath is computed very quickly Store video result In dialog box Zlevel.2, click icon Associate Video Result to Machining operation Click OK in message box Manufacturing Information Click OK to end simulation Lock Program Activate contextual menu of 3-Axis PROGRAM Select 3-Axis PROGRAM object / Lock Children Page 97

98 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Create new Manufacturing Program Click icon Manufacturing Program In the PPR tree, select 3-Axis PROGRAM The new program is inserted after it Activate Hole features Double-click Part Insert_1 in the viewer New current workbench is Part Design In PartBody, activate contextual menu of Remove feature ExplodedHoles This feature has automatically been created before in workbench Mold Tooling Design thanks to function Tools/Explode Holes which has converted the original individual Remove features into features of type Hole Select ExplodedHoles object / Activate Zoom in to briefly review the holes There are holes coming from Cooling pipes, Screws and Ejectors Page 98

99 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Go back to Manufacturing workbench In the PPR tree, double-click 3-Axis PROGRAM Click icon Update You can see in the tree that all previous 3-Axis operations need to be updated, but thanks to Lock capability, the tool paths are not lost. Run macro script to define manufacturing patterns associated to the holes Select Tools / Macro / Macros Click button Select Select file \Step7- Manufacturing\Begin\AllHolesPatterns. CATScript Click button Run Page 99

100 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Run macro script to define manufacturing patterns associated to the holes Click OK in message panel requesting Part selection Select the Insert in the 3D Viewer Click OK to acknowledge the message displayed to confirm selection Click OK to acknowledge the message indicating the end of execution Check the result Click icon Manufacturing View Activate in contextual menu : Manufacturing View object / Sort by Patterns A Machining Pattern has been created for each type of Hole Page 100

101 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Load drilling operations from existing catalog Click icon Open Catalog Double-click chapter DRILLING Define drilling for the first Cooling pipe Double-click item Machining Process.1 In the PPR tree, select newly created Manufacturing program Insertion level information is updated in dialog box Insert Object In the Manufacturing View, select the last pattern whose name is Holes_Diam10_Blind_Counterbored Click OK in dialog box Insert Object Page 101

102 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Define drilling for the second Cooling pipe In dialog box Catalog Browser, doubleclick item Machining Process.1 In the PPR tree, select operation Counter Boring.1 resulting from previous definition Insertion level information is updated in dialog box Insert Object In the Manufacturing View, select second pattern named Holes_Diam10_Blind_Counterbored Click OK in dialog box Insert Object Click Close in dialog box catalog Browser Click Close in dialog box Manufacturing View Page 102

103 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Compute the tool paths In the PPR tree, multi-select all the operations defined in Manufacturing Program.2 In contextual menu, activate Compute Tool Path Click OK in dialog box Computation mode Click OK in message dialog box to acknowledge the warning message All tool paths are now computed Page 103

104 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Display the tool paths In the PPR tree, multi-select the last three operations defined in Manufacturing Program.2 Click icon Tool Path Replay In dialog box Counter Boring.2, click icon Go to start of tool path Click icon Forward replay Simulation of operation SpotDrilling.2 begins After a few seconds, move the speed cursor right to accelerate simulation All operations are successively displayed When the simulation is finished, click OK in dialog box Counter Boring.2 Page 104

105 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Minimize the number of tool changes In the PPR tree, select Manufacturing Program.2 Click icon Auto Sequence Deactivate all options except the first one : Sort by operation type Click OK in dialog box Auto Sequence In the PPR tree, review the new sequencing Page 105

106 Step 7 : 2.5- & 3-Axis Manufacturing Define Drilling Operations Check final result with Video simulation In the PPR tree, select last operation : Counter Boring.2 Click icon Tool Path Replay In dialog box Counter Boring.2, click icon Video from last saved result Click icon Forward replay After a few seconds, move the speed cursor right to accelerate the simulation When simulation is finished, click OK in dialog box Counter Boring.2 Close without Save End of Step 7 Result data of Step 7 : \Step7-Manufacturing\End\ CompleteMachining.CATProcess Page 106