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Mold Design

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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

ME 5221 Computer-Assisted Product Realization: Lab
ME5221 Tutorial: Introduction to Pro/MOLDESIGN Pro/E Wildfire 2.0 Intent The goal here is to introduce the injection molding mold design process by providing a mold design exercise and a set of step-by-step instructions to carry out the exercise. The task is to create two mold plates for the molding of a part (solid model) that is provided. The mold plates are the parts that then can be used in the generation of machning programs for producing the mold. This tutorial is viewed as a starting point that interested individuals can use to investigate all facilities. Only some important mold characteristics and procedures are described here. Overview The general mold design procedure is - starting with a part model, a workpiece model and an empty mold creation space provided by the proMOLDESIGN program create an assembling of the reference/part model(s) and the workpiece model(s) include and check draft account for shrinkage, either by individual dimensions or isotropic shrinkage define parting surfaces(s) and volumes extract the mold volumes from the model that can be used in mold production/machining these are the mold plates extracted from the overall mold model add gates, runners, cooling lines assemble mold and mold base, etc. check for mold opening interference add ejector system And, with the mold plate models the machining programs can be developed. This exercise involves - assembling a design part and workpiece into a mold assembly, - shrinking the part model, - defining parting surfaces to use in splitting the mold, - extracting mold components to obtain a part model and mold plate models. Manufacturing Models The Part or Design Model is the model based on intended function of the product. The Reference Model includes manufacturing process specific characteristics and features needed for the part production process, e.g., draft, shrinkage consideration, etc. In a rough sense it's a model of the mold cavity. The reference model is assembled with the Workpiece Model to form the Mold Assembly. This occurs in an initially empty space provided by the program when the manufacturing part of the software is started.

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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria... The reference model can be a separate model or the design model can be designated to be the reference model. During design - changing the Reference model/part does not change the Design part, - changing the Design model changes the Reference part. Components and features can be extracted from the mold model and used, e.g., a mold plate model can be used in Pro/NC to create toolpaths and generate code to machine the component.

The two models to be used are the design model shelf2004.prt and the workpiece model workpiece_mold.prt which are Pro/Engineer models and available under Part Files on the course web site. These parts are dimensioned in mm. The part and workpiece have to be assembled to form a mold which will "work" - that is, open and allow part ejection. So it is important to understand the molding process and the terminology used, and to have a plan about how the part and workpiece model will be assembled (part model location in the workpiece which will then be split along a parting plane to produce the two mold plates). For example, if the intent is to place the reference part model in the workpiece by aligning coordinate systems, it is logical when creating the workpiece model to include a coordinates system at the location of the parting line, either by explicitly specifying a coordinate system or extruding in both directions when using the extrude capability to create the workpiece model. Start Pro/Engineer

Mold Assembly The mold creation process starts with the empty Assembly model provided and the reference and workpiece are assembled to it. File -> New... Manufacturing -> Mold Cavity name the moldfile and OK in New dialog box
MOLD menu and Mold Cavity toolbar become available A coordinate system with feature/operation planes is supplied

This is a starting feature system into which the reference part and the workpiece will be assembled and then split to create the mold model. Especially note the coordinate system and origin location as these will be used in placing the mold components (reference model and workpiece model) to form the mold. Main_Parting_Pln Pull_Direction is the direction in which the mold opens, it's probably the positive z-direction Mold_Front Mold_Right Edit -> Setup Units in ASSEM SETUP menu choose system of units to work in Set OK to warning
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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

Close Units manager Done in ASSEM SETUP Mold Model in MOLD Assemble in MOLD MODEL Ref Model in MOLD MDL TYP in the Open dialog box, select the file for the part model and Open especially note the part model coordinate system as it will be used for aligning part and workpiece models and assembly space starting the assembly process with the part model in the Component Placement dialog box choose the type of placement - and to use coordinate systems pull down the Constraint Type list and choose Coord Sys with (preselected) Select in GET COORD S pick/click on the reference part coordinate system and then the mold coordinate system OK in Component Placement dialog box if Placement Status is Fully Constrained To copy design part to reference part Merge by Ref and OK in Create Reference dialog box OK in the Create Reference Model dialog box continuing by assembling the workpiece model Mold Model in MOLD Assemble in MOLD MODEL Workpiece in MOLD MDL TYP in the Open dialog box, select workpiece file and Open in the Component Placement dialog box choose type of placement, and to use coordinate systems pull down the Constraint Type list and choose Coord Sys click on the workpiece coordinate system and then the mold coordinate system (this may be listed as a PRT_CSYS_DEF) OK in Component Placement dialog box if Fully Constrained Assess alignments, pull direction, parting plane, etc. Evaluate coordinate systems, MAIN_PARTING_PLN, etc., to assure process/mold opening will work. Done/Return in MOLD MODEL Shrinkage

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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...
The part produced will be smaller than the mold cavity since plastics shrink on cooling and solidification. Accounting for shrinkage can be included in the reference model in several ways. In the shrinkage facilities a shrinkage feature is created and applied to the reference model. The shrinkage factor, S, is used to specify shrinkage - positive value to generate a larger reference model, and hence larger mold cavity. Shrinkage can be based on the original geometry using the formula (1 + S), or based on resulting geometry using the formula (1 / ( 1 + S )) SHRINKAGE by Dimensions - applies to the design model, - can specify different shrinkage in individual, different dimensions, - individual shrinkage values override overall model shrinkage value. SHRINKAGE by Scale when done in MOLD mode the shrinkage feature is in the reference model, not in the design model, when done in PART mode the shrinkage feature is created in the design model.

For Shrinkage by Dimensions Shrinkage in MOLD By Dimension in SHRINKAGE preselected 1 + S for Formula in Shrinkage by Dimensions dialog box
note that formula is 1 + S, so shrinkage ratio may be negative

All Dimensions enter ratio to specify shrinkage
Note that individual dimensions can be manipulated in By Dim - display dimensions, set shrinkage by pick/click on dimension and supply shrinkage ratio S - for each dimension

green checkmark to accept
mold is displayed with shrunk/expanded reference part - Set/Reset in SHRK BY DIM can be used to change shrinkage

- shrink information is available Shrink Info in SHRINKAGE Done/Return in SHRK BY DIM Done/Return in SHRINKAGE To Apply Shrinkage by Scaling MOLD -> Shrinkage By Scaling in SHRINKAGE preselected 1 + S for Formula in Shrinkage by Scaling dialog box Isotropic enter Shrink Ratio PRT_CSYS_DEF:F1 to specify use of part coordinate system pick/click on model coordinate system green checkmark - shrink information is available Shrink Info in SHRINKAGE
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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

Done/Return in SHRK BY Scaling Done/Return in SHRINKAGE

Creating Parting Surface(s)
Create a parting surface parallel to mold face. This plane will be used to define (separate) the workpiece into two mold plates. Parting surfaces are useful - define parting surface and use it in splitting workpiece along it - can also use parting surfaces to split a volume --- e.g., split the workpiece into one or more volumes instead of creating the volumes Parting surfaces must be created before they are used. Regarding parting surfaces; - finished parting surface must completely intersect workpiece or volume to be split - parting surface cannot intersect itself Of the methods for creating parting planes perhaps the most useful are Copy - is handy since this uses an existing plane, Extrude - can be used to create a complex parting surface, e.g., extrude a line Offset - create a plane offset from an existing plane.

Example use of extrude MOLD -> Parting Surf -> Create enter name for the parting surface and OK in Parting Surface Name dialog box Add in SURF DEFINE (preselected)Extrude in SURF OPTS Done in SURF OPTS Done in Attributes, since defaults can be used create a plane larger than the mold plate by creating a line and extruding it across the mold/workpiece
define a sketching plane on a mold face, (preselected) Setup in SETUP SK PLN, Plane in SETUP PLANE, Pick in GET SELECT pick a workpiece surface to sketch the line on that will be extruded across the work surface to form parting plane and either use the direction shown OK or Flip (preselected) Top in SKETVIEW, Plane in SETUP PLANE, Pick in GET SELECT the prompt is to pick reference planes Close the Reference information box when Fully Placed draw a line across the mold face, Sketch -> Line draw a line completely across and extending past the ends of the workpiece Done in Sketch extrude the line across the mold to create the parting plane, (preselected) Blind in SPEC TO Done in SPEC TO specify extrusion length - larger than workpiece size OK is Surface: Extrude information box

Done/Return in SURF DEFINE Done/Return in PARTING SURF

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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

Mold Volumes, Mold Components - Splitting the Mold
To define mold volumes a parting plane is needed and it should be parallel to one of the mold faces. The definitions used in Pro/Mold are that; - mold volumes have no solid material, they are surfaces that define a closed volume in space. Volumes are intermediate steps in the process of moving from workpiece and reference model geometries to solid mold components. - the mold is constructed by building volumes and filling them with material. This is done in the Extract part of the process. - extracted components retain associativity so if a volume is modified the component is updated on regeneration of the mold model. Splitting does not alter the workpiece - the system copies the workpiece into one or two volumes that can be used for creating mold components. Spitting reproduces the volume(s). Extract is used to create the mold components after splitting. Splitting can be done using a surface, a parting surface or a volume. In the Split operation the system, - calculates the volume to one side of the parting surface, - converts the split-off volume into a mold volume, - subtracts (trims) the volume of the reference part from the workpiece geometry copied. Since volumes that do not modify existing geometry are created, a one-component split allows for extracting parts of the workpiece/mold without altering the original workpiece. So, it is possible to create a mold cavity in the workpiece by - split the workpiece to one volume, i.e, copy the workpiece to one volume, - and the system trims the reference part from the geometry copied, - resulting in a solid with the mold cavity in it. Then, split the resulting solid into two volumes at the desired parting plane(s)

To Split to Two Volumes MOLD -> Mold Volume Split in MOLD VOLUME (preselected) Two Volumes and All Wrkpcs in SPLIT VOLUME Done in SPLIT VOLUME with preselected Pick in GET SELECT, or use of Select by Menu which may be easier select the parting surface, (it must intersect the entire workpiece and not be blanked)
for more complicated molds it may be useful/necessary to create and use more than one parting plane

Done Sel in GET SELECT OK in Split dialog box
system computes the two volumes, highlights each in turn and prompts for new names

enter volume names for the two volumes sequentially in the Volume names dialog box and OK Done/Return in MOLD VOLUME To make the resulting volumes into solid mold components - for both volumes MOLD ->Mold Comp Extract in MOLD COMP select volume desired in Create Mold Component dialog box and OK

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Pro/MoldDesign same procedure for other volume

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

Done/Return in MOLD COMP and on Save mold halves are now solid models (
To Split to One Volume

MOLD -> Mold Volume -> Split One Volume and All Wrkpcs in SPLIT VOLUME
if mold volumes already exist would have to choose the features of interest from choose All Wrkpcs, Mold Volume or Sel Comp

Done in SPLIT VOLUME the Split dialog box opens select an existing parting surface to use to split the workpiece
if failure occurs must use Show Errors -> Item Info

select the island to include (moving the cursor over island list highlights islands) OK in Split enter name of new volume and OK in V olume Name dialog box Done/Return in MOLD VOLUME To turn the resulting volumes into solid mold components MOLD ->Mold Comp Extract in MOLD COMP select volume desired in Create Mold Component dialog box and OK Done/Return in MOLD COMP

) Mold Opening MOLD -> Mold Opening Define Step in MOLD OPEN Define Move in DEFINE STEP select the part of the mold model that moves on mold opening, say by Sel By Menu in GET SELECT, choose the mold component, Select in Selection Tools dialog box Done Sel in GET SELECT To select motion direction, say by (preselected)Define Move in DEFINE STEP, Pick in GET SELECT pick a mold edge, or coordinate system direction, etc. enter a move distance Done in DEFINE STEP Done/Return in MOLD OPEN Mold Opening in MOLD, Done/Return in MOLD OPEN

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Pro/MoldDesign

http://www.me.umn.edu/courses/old_me_course_pages/me5221/Tutoria...

Adding Mold Features - Water Line
Mold features are needed to complete the mold, e.g., draft, runners, ejector system, etc. As an example, to add a water line - define the water line diameter, - specify the water line by sketching a line between water line end points, --- this requires creating a sketching plane on which to draw the water line path. One way to create a sketching plane is by offset, and for a water line offseting the sketching plane from the mold parting plane is logical. in the Tool Bar Insert -> Surface -> Offset select the surface to offset from, by, say Sel by Menu in GET SELECT choose the parting surface and Select in Selection Tools dialog box the selected plane that the new plane is to be offset from is highlighted choose direction of offset in SURFACE: Offset dialog box enter offset distance in SURFACE: Offset dialog box and the green checkmark The offset plane is added and can be used as the sketching plane for the water line.

To create a water line Feature in MOLD Cavity Assem in MOLD MDL TYP Water Line in MOLD FEAT enter water line diameter Sketch a line between the end points of the water line to pick the sketching plane
(preselected) Setup in SETUP SK PLN, Plane in SETUP PLANE, Pick in GET SELECT - pick the plane to sketch the line on that will be the water line - and either use the direction shown OK or Flip Top in SKETVIEW, Plane in SETUP PLANE, Pick in GET SELECT the prompt is to pick reference planes Close the Reference information box when Fully Placed

draw a line across the mold face,
Sketch -> Line draw a line for the water line completely across the workpiece/mold plate Done in Sketch

Auto Add in Intersected Comps dialog box since default are useable OK in Intersected Comps dialog box Done/Return in FEAT OPER

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