Week 9 - Project 1 - Door Trim Lower with Engineering Features

Objective:

• The main aim of this challenge is to create a solid body of 'Door Trim Lower' with the help of the closed surface method by using the 'Generative shape design' workbench in CATIA V5. Performing the 'Draft Analysis' on the solid part body of the Door trim.

Given sample design

Overview:
Initially, we need to offset the given Door Trim class A surface in the inner direction to the required thickness (here the thickness is 2.5mm). After that, we need to close the patches on the offset surface of the bumper, the patches are formed due to the fillets on the Class A surface. Once all the patches are closed properly join them together to make a proper class B surface and now sweep the boundary of the class A surface to trim with the class B surface to make a closed body. By using the closed body command in the Prat workbench we can get the solid body from the closed surface of the Door Trim. Now, I created the Heat stakes and Locators by considering all the design parameters. After creating all the B-side features on the solid part body of the door trim, I performed a draft analysis for it to check whether all the surfaces are drafted properly or not (The draft angle for the plastic component is 0.5deg to 3deg).

TOOLING AXIS:

To create the tooling axis, I extracted a surface from class A and created a point in the middle of the surface by using the point command and created a line at that point through the x-axis. Now, I performed a draft analysis check from that line whether the created tooling axis is in the correct position or not. If in the draft, analysis check the surface highlighted with green colour on both sides of the surface the tooling axis is in the correct position and direction.

Tooling axis:

DRAFT ANALYSIS FOR CLASS A SURFACE:

We do perform the draft analysis check for class A surface before we make solid and creation of B-side features. Initially I align the compass to the tooling axis and I gave a 3deg draft angle for the green colour in the colour bar. If the surface is highlighted in green colour the draft angle is given properly for class A surface. If the class A surface is not highlighted fully in green colour, that might be the reason for the draft angle of the class A surface.

CLASS B SURFACE:

To create the class B surface, offset the class A surface inside as per our thickness requirement (here the thickness is 2.5mm, so I offset the class A to 2.5mm inside). Once the offset is created, we can observe some patches on the offset surface by taking the boundary for the offset surface, those patches are formed due to the fillets on the class A surface. We need to cover those patches with the help of the multi-section surfaces command by extracting the patch boundaries. Once all the patches on the offset are covered properly join all the patches with the offset surface, to get the replicated surface of the class A surface.

CLASS C SURFACE:

I used the sweep command to create the class C surface concerning the boundary of the class A surface. Initially, I extracted the boundary of the class A surface with tangent continuity, and I sweep the extracted boundary concerning the surface at 93deg (for draft angle) for 4mm to intersect properly with the class B surface. Once we sweep all the surface boundaries of class A, extrapolate the sweeped surfaces until both surfaces got intersect properly, and trim them to remove extended extrapolated surfaces to get a proper sweep boundary throughout the entire surface, including the centre hole of the door trim. Now, join both class A and sweep boundary to get the complete class C surface.

PART BODY:

To create the solid part body from the closed surface, I used the closed surface command in the part workbench.

CREATION OF LOCATORS:

To create the locators, I created a sketch on the body. After creating the sketch, I pad it 20mm in height and thicken it to 1.3mm and I drafted it with 0.5deg in the direction of the tooling axis. I gave 5mm of chamfer with 45deg of inclination and after I gave a fillet of 0.25mm radius.

4-way locator:

CREATION OF HEAT STAKES:

To create the heat stakes, I draw a sketch on the surface. After the creation of the sketch, I pad it to 18mm height and I gave a draft angle of 0.5deg on both sides (inside and outside) and then I gave a fillet with a 0.25mm radius. After creating the heat stake, I created the ribs for supporting purposes. To create the ribs, I draw a sketch and padded it to 12mm in height and 1mm in thickness. After padding the ribs, I drafted 0.5deg in the tooling asix direction and filleted it with a 0.25mm radius. Finally, I union trim the ribs with a heat stake to remove the ribs, which are present inside the heat stakes.

Heat stake with supporting ribs:

Now I Power copy the heat stakes by giving inputs like point and plane copy them in the part body according to the requirement.

Final part body with 4-way locators including all the heat stakes with supporting ribs:

CREATION OF RIBS:

Ribs are a feature in plastic injection molded parts. They are thin extensions that run perpendicular from a wall or plane. They are commonly used to provide additional support and strength to a part. Thickness and location are essential to rib design.

To create the ribs, I draw a sketch and padded it to 12mm in height and 1mm in thickness. After padding the ribs, I drafted 0.5deg in the tooling asix direction and filleted it with a 0.25mm radius.

use power copy to produce rib and another two ribs are produce using tranlate command to have command on both the steps.

CREATION OF DOG HOUSE:

Dog house is an engineering feature used in plastic trim design. Dog houses are used as supporting feature. Sometimes other engineering features like snaps; locators etc. are mounded on them to increase their strength.

• To create the Dog house, I draw a sketch and padded it to 18mm in height .
• After padding in the direction of tooling axis, I drafted 3deg in the tooling axis direction and filleted it with a 3mm radius.
• Than i remove the material from the base of it having a thickness of 0.4*T=1 mm.
• Than provide draft it to 0.5degree in the direction of side core axis.
• Then shell the main padded structure to 0.7*T=1.75mm.
• Remove the second bbody from the first body .
• After joining both the bodies translate it to required points and rotate it with respect to its edge .

• After producing all the dog house unitrim it with the solid surface previously produced.

the final produced solid body having all the fetures is shown below..

DRAFT ANALYSIS FOR PART BODY:

FOR 3 DEGREE D

FOR 0.49 DEGREE

PROCEDURE:

1.Check for any openings in the given model Door Applique by using BOUNDARY. In BOUNDARY > select edges - select the surface to create the boundary at the openings.

2.Create a point at the center of the surface by using Point Definition by : Point Type - on surface ,Surface - select the surface and Distance - 0

3.By using the Line Definition option create a line in Y direction by : Line Type - Point-Direction, Point - select the point and Direction - Y which will be the Main Tooling Axis(Yellow).

4.Do the draft analysis on Class A surface.

CREATING B-SURFACE FOR DOOR APPLIQUE:

5.Extract the Class A surfaces by selecting the surface to extract and Untrim the surfaces by selecting the surfaces which are required and offset the untrimmed surfaces by selecting the surfaces to offset to a distance of 2.5mm and then trim the surfaces.

6.Fillet the surface with a radius and extrapolate the surface.

CREATING C-SURFACE FOR DOOR APPLIQUE:

7.Extract the Boundary of Class A by Extract option and Using Sweep option create the Class C surface.

8.Smooth curve the extracted boundary and then in Sweep option : Type - With draft direction , Guide Curve - Boundary and Draft direction - Tooling axis and angle as 3 degrees.

9.Create the C surface for 2 boundaries separately.

10.After creating the C surface,join the Class A and Class C surface by Join option and then trim it with the B surface.

11.In Part Design,fill the surface body with the solid using Close surface.

ADDING LOCATORS(4 WAYand 2 WAY) TO DOOR APPLIQUE:

12.Create a point at the center of the surface of Door Attachment by Point Definition.

13.Create a plane on the surface at the center by Plane Definition with reference to the Point which was created and then create a sketch of a 4 way locator on the plane.

14.Pad the Sketch in Part Design, in Pad : Type - to surface , Limit - select the surface as limit and Profile - Sketch and in Pad tick mark the “Thick” option and then click the more option and select the Neutral fibre and the thickness 1 should be 40% of the main wall thickness.

15.Draft the faces of the padded area by Faces to draft - select the faces to draft , Neutral element selection - select the base surface and pulling direction - Tooling axis.

16.After drafting the faces,chamfer the edges at the top and Objects to chamfer - select the edges , Mode - Length/Angle.

17.Fillet the edges and faces.

18.Copy the Part body of the 4 way Locator and Paste it Special with reference link and then Translate it to the other side by coordinates by Translate option : Vector Definition - Coordinates.

19.Now create a 2 way Locator at below the center by creating a sketch and do the same process of Padding,Drafting,Chamfering and Filleting.

20.By Boolean operation,Unitrim the Locators with the Solid body of Door Applique by selecting the faces to keep.

ADDING HEAT STAKES TO DOOR APPLIQUE:

21.Offset the Class A surface to 2.5mm and extract the boundaries of the offsetted surface.

22.Parallel Curve the extracted boundaries by Parallel Curve Definition : Curve - extracted boundary, Support - surface , Constant - distance.

23.Give the Points Repetition to the Parallel curves by Points and Planes Repetition by : Curve - Parallel curve, Parameters - Instances and Instances - no of points.NO Heat stakes should present nearer to Locators.

24.Now create a sketch on the point created on a Parallel curve.Draw the circles with diameters of 5mm and 7mm and in Part Design,Pad it : Type - to surface , Limit - select the Class A surface.

25.Copy the Part body of the Heat Stake and Paste it Special with reference link and then Replicate to the points which are created by Translate option : Vector Definition - Point - Point.Translate the part body of Heat Stake to the other point which was copied by selecting the start point and endpoint.

26.By Boolean operation,Assemble all the Heat stakes part bodies in a single body and then Unitrim the Heat Stakes with the Solid body of Door Applique by selecting the faces to keep.The distance between the tip surface of locator and Door Attachment surface should be equal for all locators.Also the height of Heat stake should be smaller than the Locators.

THICKEN THE DOOR ATTACHMENT SURFACE AND CREATING CLEARANCES FOR LOCATORS AND HEAT STAKES

27.Thicken the Door Attachment surface by Thicken option in Part Design by selecting the surface to thicken to 2.5mm.

28.Now from the Locators sketch,copy the sketch into a new geometrical set and then draw a circle of 15mm and make the old sketch as construction lines where making the clearance for Locators.

29.Pad the circle to an offset distance below the Door Attachment surface and draft the surface to 0.5 degrees.

30.By Boolean operation,remove the Pad from the Thicken surface.So the clearance gap between the Locator wall and clearance wall should be 0.1mm to lock the motion.

31.Do the same process for remaining Locators and Heat stakes by creating the Clearance gaps where the Clearance gap for Heat Stake should be 0.5mm.

32.Finally do the Draft Analysis for the final component

RESULT:

• Create the Plastic design and attached the Engineering features and generated the Draft Analysis for the given Door Applique Class A model.