Challenge

Week 12- Final project

SSunny Kumar23 Jul 2023

OBJECTIVE

Create the Door Trim Assembly from the given A Surface.
Refer to the Master section for Nominal thickness, Flanges, and Heatstakes.
Assemble the respective components into one single Product:
- Straight Arm Rest
- Inclined Arm Rest
- Upper Map
- Lower Map Pocket
- Lower Substrate

PROCEDURE

STEP 1: ASSIGNING A SURFACE and MASTER SECTIONS

*Visually*	*Using the Join option. This option is efficient but not effective.*
*Manually*	*Extracting the Boundary of the Class A surface. This option confirms better.*

The Input file has a single Geometric set with all the surfaces of the Class A Door trim.
We have to extract and assign the respective surfaces to each component.
We extract the A surface for the following components:
- Straight Arm Rest
- Inclined Arm Rest
- Upper Map
- Lower Map Pocket
- Lower Substrate

PART NO.	INSTANCE NAME	CLASS A
PART 1	Straight Arm Rest

PART 2	Inclined Arm Rest

PART 3	Upper Map

PART 4	Lower Map Pocket

PART 5	Lower Substrate

STEP 2: CREATE ASSEMBLY

Collect the parts inside one assembly (Create a New Product), by either of the options:

Copy + Paste
Add Existing Component

Save Management:
- We cannot directly save the file by pressing Ctrl+S, because we have to organize the parts in the assembly file folder.

File > Save Management > Select the Parent Product > Save As (Create a separate folder) >

STEP 2: FIND THE TOOLING AXIS

Tooling Axis is the direction in which the Mold(Core-Cavity) travels perpendicular to the parting surface/line.
Place the component on each plane (XY/YZ/ZX) and find the desirable tooling direction.

[Note: The plausible tooling axis is perpendicular to a Hole or large flat surface so look for those features when selecting.]

So we need to create a midpoint on the plane perpendicular to the tooling axis.

Holes	Use Multiple extracts to get the Boundary and define a midpoint using the "Curve/Circle" option.
Flat Surfaces	Extract the surface and then create a mid-point using the "On Surface" option.

Now, introduce an Axis system at the Midpoint. This will act as a reference coordinate system.

STEP 4: DRAW THE TOOLING/DRAFTING AXIS

Due to the complexity of the geometry, the Bisecting method won't be accurate and also takes too much time and effort.
Therefore, it is best to go with the Compass Method:
- Insert > Analysis > Feature Draft Analysis
- Simply place the compass on the largest flat surface.
- Check the Analysis.
- Tilt the Compass by Orientation or Rotation about an axis to get the desired result.
After finalizing the orientation, lock the compass direction.
Create a Line, this will be our Reference Axis:
- Line > Point-Direction > Select Point > Select Direction (Compass Direction)

Colour	Description	Value
Green	Core Side	Above 3 degrees
Blue	Parting Line	0 degrees
Red	Cavity Side	Below 0 degrees

PART NO.	INSTANCE NAME	MAIN TOOLING	SIDE TOOLING
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

ADVANTAGE OF COMPASS METHOD:

We can define the Tooling direction and conduct a draft analysis simultaneously from within the "Feature Draft Analysis" Tool.

NOTE:

If there are no flat surfaces, then use the "Measure Inertia" tool to get the Centre of Gravity and the Axis System for the selected complex geometry.
If some regions fail for draft analysis, then we have to introduce a Lifter/Side Core as well.

STEP 5: A SURFACE FLANGES

From the given Master section, we have to create the Flanges and join/trim them with the A surface input to create one single Entity.
Operations performed in creating Flanges:

*EXTRACT*
*SWEEP*
*EXTRAPOLATE*
*TRIM/SPLIT*
*JOIN*

The newly edited A surface with Flanges will be our new input for creating the Solid component.

STEP 6: B SURFACE CREATION

Note: Depending on the geometry, the extraction and offset of the fillets might generate non-uniform thickness. So it is advisable to extract only the flat surfaces and then apply fillets at the end of Class B formation.

Perform the following operations in the order:

EXTRACT	Choose the respective A surface and extract with no propagation option.
UNTRIM	The extracted surface will possess the specific trimmed. Untrim to get the basic geometry.
EXTRAPOLATE	The surfaces have to overlap each other in order to facilitate trimming therefore extrapolate it up to the required dimension.
TRIM	Trim the surfaces according to the required geometry.
OFFSET	Now, Offset the Trimmed geometry by the value of the thickness of the component. This Offset is our B Surface. Note: Offset the Silent Fillet separately and then trim with the bucket
FILLET	Extract the Fillet surface from Class A. Untrim to get the basic Geometric shape. Measure the uniform radius of the surface. Apply Fillet to the respective edges to get the desired finish.

Note: The fillet radius of the Class B offset is altered to maintain the uniform thickness throughout the geometry.

Offset direction	Fillet Radius
Inward	Initial Radius - Thickness
Outward	initial Radius + Thickness

PART NO.	INSTANCE NAME	B SURFACE
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

STEP 7: C SURFACE CREATION

C surface is the part of the geometry that connects Class A with B surface.

Rules to be followed. for C surface creation:

A minimum draft of 3 degrees should be provided to facilitate the Ejection of the Molded component.
The parting line should be on the B surface. This means that the draft should sweep outwards, from the C surface.

Perform the following operations in the order:

MULTIPLE EXTRACT	Extract only the Boundary by Tangential selection.
CURVE SMOOTH	We need minimum Parting lines as possibles, so smoothen the extracted boundary.
SWEEP	The C surface is swept with the Line option along the Drafting Angle Direction. Guide Curve: Select the Smoothened Curve Draft Direction: Select the Tooling Axis Draft Angle: 3 Degrees
MULTI-SECTIONS SURFACE	In places like Fillets where the Sweep option doesn't work, we can fill in the gap using MSS. Choose the Sections. Then choose the Guide Curve along which we can drag the profile.
EXTRAPOLATE	The Sweeps at the edges need to overlap in
JOIN	For our future reference, we can Join all the C surface sweeps as one single entity.

PART NO.	INSTANCE NAME	C SURFACE
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

STEP 8: CLOSED SURFACE

First Trim/Join Class A with Class C.
Then Trim with Class B and keep the respective surfaces.

PART NO.	INSTANCE NAME	CLOSED SURFACE
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

STEP 9: CLOSED BODY DRAFT ANALYSIS

All the 3 class surfaces must pass in this analysis.

Insert > Analysis > Feature Draft Analysis

Note: Ensure you have the Material view mode ON.

Define the Draft direction using the "Compass" option.
- Drag the Axis system representation close to the model and align it along the tooling axis.
"Lock" the Draft direction.
Set the Colour scale

*Colour*	*Description*	*Value*
*Green*	*Core Side*	*Above 3 degrees*
*Blue*	*---*	*0 degrees*
*Red*	*Cavity Side*	*Below 0 degrees*

Place the Analysis Tool (Arrow Icon) anywhere on the model and review the colours on the feature.
If any feature (especially C surface) is showing Blue/Red then choose the same option again (It will switch to Analysis under Running point) and place it on the respective feature to review the deviation of the sweep angle from the Tooling Axis.

STEP 10: PLASTIC FEATURE: DOG HOUSE

DEFINITION

It is a feature used:
- To avoid sink marks.
- Solve length issue.
- Provide strength and assembly.

DESIGN GUIDELINES FOR DOG HOUSE

*Draft*	*Outer Draft ≥">≥≥3 Degree`* *Inner Draft ≥">≥≥ 0.5 Degrees*
*Width*	*Top face width ≥">≥≥ 11 mm`* *WidthHeight">WidthHeight��ℎ��ℎ�= 31">3131*
*Sink Saver*	*Parting wall Thickness, C ≤">≤≤40% T* *Parting wall Height, B = 3 to 6 mm*

Operations performed for creating Doghouse:

*1.1*	*Extrude*	*Create a straight line sketch using the surface as support.* *In the Surface workbench, Extrude the line in the direction of the Tooling axis.*
*1.2*	*Trim*	*Trim the surfaces according to the required geometry.*
*1.3*	*Thickness*	*Go to the Part workbench and add Thickness to the extruded surface.* *We now have a solid rib of definite volume and density.*
*1.4*	*Draft*	*Give Draft of 0.5-1.5 degrees on all the vertical faces of the rib.* *This is done for easy ejection of the Core and to avoid any damage to the molded component.* *Select the faces to draft, neutral element, and pulling direction.*

Operations performed for creating Sink Saver:

*2.1*	*Multiple Extract*	*Extract the inner faces of the dog house.*
*2.2*	*Extrapolate*	*The surfaces have to overlap each other in order to facilitate trimming/splitting therefore extrapolate it up to the required dimension.*
*2.3*	*Offset*	*Offset the faces to provide a parting wall thickness.* *C ≤">≤≤40% T*
*2.4*	*Split*	*Split the offset with the thickened dog house in the part workbench.*
*2.5*	*Fillet*	*We provide rounded corners at edges to facilitate easy flow rate and avoid Flowlines.*

STEP 11: PLASTIC FEATURE: PUSH PIN

DEFINITION

It is a feature that facilitates:
- Locating and Arresting components of an Assembly.
- Providing Alignment in Mating Parts.
- Acting as a stopper or guide for various mechanisms.

DESIGN GUIDELINES FOR PUSH PIN

Operations to be followed:

*Positioned Sketch*	*Draw the Boundary of the sketch to be revolved.*
*Revolve/Shaft*	*Revolve the sketch about it's axis.*
*Pad*	*There are some slots in the revolved geometry to facilitate as guideway for locating and arresting.* *Create a Rib sketch and then Pad it.*
*Boolean Remove*	*Remove the Padded rib from the revolved geometry to get the desired shape of the pushclip.*
*Chamfer*
*Fillet*	*We provide rounded corners at edges to facilitate easy flow rate and avoid Flowlines.* *Min. Radius = 0.25*

STEP 12: PLASTIC FEATURE: HEAT STAKE

GUIDELINES FOR HEAT STAKE DESIGN

Diameter	There are no standards for Dia, it depends on the manufacturer. The dimension is altered in such way that sink marks are avoided.
Thickness	There is no standard for thickness as well, but keep it lesser than the part thickness. Minimum 0.75mm at the Tip of the Rib. Molten material won't reach any further.
Height	Height of Heatstake < Height of Locator Since Fixing occurs after Locating.
Draft	0.5 degree.
Flat plate	Dia of Flat Plate = 2.5 x (Dia of Heat Stake).
Clearance	0.1mm to accommodate for clearance.
Spacing	65-100 mm

GUIDELINES FOR RIB DESIGN TO SUPPORT HEAT STAKES

Draft	0.5-1.5 Degrees If it is more, then the rib will be too narrow at the top and mold wouldn't fully fill the rib.
Thickness	(0.4-0.5) T at the base of the rib. The larger the area of the base of the rib, the more heat retained. Retained heat causes more shrinkage. This leads to Sink marks as well. Minimum 0.75mm at the Tip of the Rib. Molten material won't reach any further.
Fillet	Maximum radius = 0.25 mm. Due to the less thickness of the rib we need to maintain a small fillet radius, or else we'll get ribbon formation.
Height	Height ≤">≤≤ 5T Taller ribs are prone to buckling.
Base Rib Root Dia	D ≤">≤≤30% of Deviation from Thickness. Greater than that causes Sinkmark.

Operations to be followed:

Extrude	Create a straight line sketch using the surface as support. In the Surface workbench, Extrude the line in the direction of the Tooling axis.
Thickness	Go to the Part workbench and add Thickness to the extruded surface. We now have a solid rib of definite volume and density.
Draft	Give Draft of 0.5-1.5 degrees on all the vertical faces of the rib. This is done for easy ejection of the Core and to avoid any damage to the molded component.
Boolean	Boolean Add/Union Trim the Rib to the Coin holder body.
Fillet	We provide rounded corners at edges to facilitate easy flow rate and avoid Flowlines.

STEP 13: TRANSLATION OF PLASTIC FEATURES

After creating a single feature, we can translate it multiple times to the desired location.
First Copy the respective feature's part body into the main part file:
- Copy > Paste Special > As specified in Part Document
This removes the Parent-Children relationship and we can edit the translated part according to our needs.

STEP 14: BOOLEAN OPERATION

We have to add all the translated features to the Main body of the Substrate.
The Union Trim operation fit the best option for our needs.
Define the Main part body as the Working Object.
- Select Feature Body > Union Trim > Select Faces to remove/keep

STEP 15: CLEARANCE FOR HEAT STAKES PROVIDED ON FLANGES

The door trim Assembly has to be rigidly fixed as one unit.
The 4 components will be permanently arrested to the Lowered substrate by using the Heastakes.
The Heatstakes will pass through the flanges of the components, therefore some clearance of 0.1mm has to be provided.

PART NO.	INSTANCE NAME	FLANGES WITH CLEARANCE
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

STEP 16: FINAL DRAFT ANALYSIS

Insert > Analysis > Feature Draft Analysis

Note: Ensure you have the Material view mode ON.

Define the Draft direction using the "Compass" option.
- Drag the Axis system representation close to the model and align it along the tooling axis.
"Lock" the Draft direction.
Set the Colour scale

Colour	Description	Value
Green	Core Side	Above 0.5 degrees
Blue	Parting Line	0 degrees
Red	Cavity Side	Below 0 degrees

Place the Analysis Tool (Arrow Icon) anywhere on the model and review the colours on the feature.
If any feature is showing Blue/Red then choose the same option again (It will switch to Analysis under Running point) and place it on the respective feature to review the deviation of the sweep angle from the Tooling Axis.

PART NO.	INSTANCE NAME	DRAFT ANALYSIS: MAIN TOOLING	DRAFT ANALYSIS: SIDE TOOLING
1	Straight Arm Rest

2	Inclined Arm Rest

3	Upper Map

4	Lower Map Pocket

5	Lower Substrate

RESULT

The A surface of the following components converted to a solid body:
- Straight Arm Rest
- Inclined Arm Rest
- Upper Map
- Lower Map Pocket
- Lower Substrate
Each component has a uniform thickness of 2.5mm.
The components' surfaces (A, B & C) pass for Drafting analysis.
The Plastic features follow the design guidelines and pass for the Lifter draft analysis.
Clearance is provided on the Flanges, allowing for the Heatstakes to arrest and form an Assembly.