Week 12- Final project

FINAL PROJECT

AIM - To create the Door trim panel's CAD model considering the inputs given to me following the design rules and OEM standards.

ABSTRACT - The project deals with the explanation of steps and procedures followed while developing the Door Trim Panel of a car using CATIA V5. Using the class A surface I was able to create the tooling axis, class B surface, class C surface, and after forming the solid body from that I was able to create the flanges and the B side features such as Dog house, push pins, Heat stakes, etc. And finally, the draft analysis is also done on the components to check the manufacturability of the components.

INTRODUCTION - The door panel will usually match the rest of the vehicle's interior. Door panels were formerly made of cardboard with an upholstered interior finish of vinyl, leather, cloth, carpet, or other materials for the decorative trim. Modern cars typically have door cards made of plastic, most often using injection molding, as well as incorporating other decorative materials.

The design should incorporate both the necessary service amount and the functional unit (such as "it is strong" and "it looks and feels good") so that a given car door panel "would service a car body's life span of 200,000 kilometers (124,274 mi)." The door panel typically incorporates other parts that contribute to the appearance, functionality, and ergonomics of the vehicle. These include armrests, switches, or other controls for windows and the locking mechanism, convenience lights, Map pockets, lower substrate, storage compartments, and other features. An image of the door trim panel is shown below:

Class-A surface:

The Class-A surface is the outermost surface of the plastic component which is also looks fine surface and it is the aesthetic surface that the designer creates as an input part for the design work.

Class-B surface:

The Class-B finish is a quality finish with only minimal imperfections. A Class-B finish is the most common finish for exterior surfaces. It is normally specified on surfaces such as external covers, panels, and parts that are fairly prominent.

Class-C surface:

The Class-C finish allows more imperfections than Class-A or Class-B. Class-C is often specified for interior surfaces not readily visible, surfaces that will be covered by another part when assembled, or surfaces which the Customer feels do not need to meet a high cosmetic finish.

Tooling Axis:

In Molding, machine arrangement is given to open the mold along a direction which is known as Tooling Direction. In other words. The mold is built from two separate halves (Core and Cavity) and tooling direction basically defines the direction of mold or core pulls apart.

Draft Analysis:

The Draft Analysis command enables you to detect if the part you drafted will be easily removed. This type of analysis is performed based on color ranges identifying zones on the analysed element where the deviation from the draft direction at any point, corresponds to specified values. Most parts or applications require minimum of 1/2 to 1 degree, however 3 degrees is widely accepted as the norm.

Design Methodology:

Components of Door Trim panel:

1. Arm Rest
2. Lower Substrate
3. Upper Map Pocket
4. Lower Map Holder

The steps that I followed for this project is mentioned below:

1) Extracting the class A surface from the input

2) Draft Analysis of class A

3) Creation of Class B and Class C surface from Class A

4) Created the solid body and performed the draft analysis on the solid body

5) created the flanges

6) Created the Engineering features

7) Draft analysis of the component with Engineering features.

PROCEDURE - Here the input which is given to me is below:

In the above fig., u can see that the surfaces along with the master section are given to me.

Master section - Master section are the guides for a design that shapes the component after technical styling of class A surface. The Master section is parameterized model of the vehicle body that outlines the guidelines for the NPD team.

so here I have to create three parts that are mentioned below:

1) Lower substrate

2) Map pocket

3) Door Armrest

Then I have to create the attachment features that are required for the assembly of the parts.

First I have started by creating the lower substrate. For this, I have extracted the class A surface of the lower substrate from the input that is given. The extract is shown below:

The class A surface of the lower substrate is shown below:

LOWER SUBSTATE :-

Then I have split the extra portion from the class A surface by creating the line and splitting using the split feature in generative shape design. so the final class A surface is shown below:

Now I have to perform the draft analysis on the class A surface. For the draft analysis, I need a tooling axis for this lower substrate.

Tooling axis - The tooling axis is defined as the direction in which the mold opens or core and cavity opens and closes. The selection of the correct tooling axis is important to ensure the component is taken out perfectly and also the cost of the component should be less.

I will start by insering a geometrical set and naming it as a tooling direction. For creating the tooling axis I will analyze the model and see from which direction I can see the whole model. so here the direction I have chosen for the tooling axis is along y-direction because along y-direction the whole model is visible properly. For creating the tooling axis I will create one point on the lower substrate and from that point, I will create one line along the y-direction and that line will be my tooling axis. The tooling axis is shown below:

After creating the tooling axis I have done the draft analysis on the lower substrate.

Draft analysis - Draft analysis is a technique to analyze whether the component created is manufacturable or not based on the draft conditions applied. So here I will provide the direction in which the component should be ejected to get the easy removal. My dirction will be the tooling axis that I have created.

The minimum draft value for the Automotive plastic component is 3 degrees and those for the texture faces 7 degrees of the draft is suitable. The draft is provided to the component for easy removal from the mold in the case of the plastic components.

So here I will change the customize view parameters and will select the material mode.

Then I will go insert and select the analysis and in the analysis, I will select the draft analysis. The draft analysis block is shown below:

In the above fig. under the display, the section selects the color scale and turns on the light effect for proper visualization. then under the direction section, I will click on the compass and will drag the compass from vehicle zero to my tooling axis. and then I will click on the lock feature and will select the class on the surface. The result is shown below:

The color scale shown above denotes the following:

The Green color denotes that the draft provided is above 2.9 degrees.

The Blue color denotes that the draft provided is between o and 2.9 degrees.

The Red color denotes that the draft provided is negative.

After performing the draft analysis I have made sure that the proper draft is provided on the component and now I can create the further surfaces which are class B and Class C surfaces.

Class B surface - It is a surface that gives thickness from a class A surface. All the supporting features of the component will be formed on the B surface only. so we can say that Class B is an engineering surface and Class A is an aesthetic surface.

For creating the class B surface I have offset the Class A surface to 2.5 mm which is the thickness of the part according to the master section that is given as the input. The offset is shown below:

After offsetting the class A surface to 2.5 mm I have extrapolated the class B surface up to the extent to which it can be trimmed later with the class C surface. The Final extrapolated B surface is shown below:

CLASS C SURFACE - Class C surface is defined as the surface which connects the CLASS A and CLASS B SURFACE along the tooling direction. The tooling direction here will be my tooling axis.

For creating Class C I have extracted the boundaries of the class A surface and swept the extract along the draft direction. giving a 3 degrees draft. Also, I have used the smooth curve feature to smoothen the swept surfaces. Here I have also used the reference surface option in sweeping for the portion that does not require a sweep with draft direction. The sweep parameters are shown below:

Then I have joined the sweeps that I created and if some sweep is extending I have trimmed it according to my requirement to get the class C surface. The final class C surface is shown below:

After creating the class C surface I have joined it with the class A surface. The join is shown below:

Then finally I have trimmed the Join of class A and class C with class B surface to get the required part. The trim is shown below:

Then after creating I have made sure that I have a close surface. so for validating that I have to use the boundary option and clicked on the surface I got an error which proves that I have a closed surface. The closed surface is shown below:

After this, I have created a solid body from this closed surface by using the close surface feature in part design. The solid lower substrate is shown below:

Then I have performed the draft analysis on the solid part. The draft analysis is shown below:

Now after creating the lower substrate I have created the map pocket

For the map pocket, I have divided it into two parts one is the inner map pocket and the other is the outer map pocket.

OUTER MAP POCKET -

first creating the outer map pocket following the same procedures as I did for the lower substrate. So extracting the outer map pocket surfaces from the input. The multiple extracts are shown below which is also the class A surface for the outer map pocket.

Tooling axis - For creating the tooling axis again I have created the point on the surface and from that point, I created a line which is the tooling axis for the outer map pocket. The tooling axis is shown below:

Now the draft analysis on the class A surface is sown below:

Class B surface -Now for the class B surface again I have just offset the class A surface to 2.5 mm. The offset is shown below:

The offset that I got was not proper and it had some gaps so I filled that gap using the multisection surface feature in generative shape design. The multisection surface is shown below:

Then I have joined the multisection surface with the offset to get the class B surface. The final class B is shown below:

Class C surface - For creating the class C surface I have taken the boundary of class A and class B surface and blended them together. Before blending them together I have given smooth curves to the boundaries of A and B. The blend is shown below:

Then I have just joined class A, class B, and the blend which is my class C surface. The join will give the part that is the outer map pocket.

I got the part but it was not a closed boundary or closed surface so to resolve that issue I have taken the intersect between class A and Blend and another intersect between the class B and the class C surface. After creating the intersection I have split the class B and the intersect of B and C. same I have done for the c surface as well and the similar thing I have done with the intersection of A and C is have split the A surface with the intersection of A and C. Finally I have joined the splits together to get the part with a closed surface. The closed boundary is shown below:

Then after creating the closed surface I have created the solid part from this closed surface using the closed surface feature in part design. The solid part is shown below:

Then I have performed the draft analysis on the solid part. the draft analysis is shown below:

Inner map pocket - For creating the inner map pocket again I have followed the same procedures as I did before. So extracting the surfaces that form the inner map pocket. The extracted surface is shown below:

BOTTEL HOLDER :-

After multiple extracts, the surface I got was a class-A surface of the inner map pocket. The class A surface is shown below:

Now I have performed the draft analysis on the class A surface. But before that, I have created the tooling axis

Tooling axis - For creating the tooling axis I have followed the same procedure that is creating a point on the class A surface and creating a line from that point along the direction in which class A is clearly visible. The tooling axis is shown below:

The draft analysis is shown below:

Now I have created the other two surfaces.

Class B surface - For class B again I have offset class A to 2.5 mm. The offset is shown below:

Class C surface - For creating the class C again I have swept the boundaries of class A using the 'with reference surface' option in the sweep command. And I have swept the boundaries to 87 degrees with the reference surface of the boundaries. The sweep parameters are shown below:

Then I have joined all the sweeps that I created to get the class C surface. The class C surface is shown below:

Then I have joined the Class A and Class C surfaces. The join is shown below:

Then I have trimmed the join of A and C with class B surface after extrapolating the class B wherever it's required. The Trim is shown below:

After creating the part I have checked the surface whether it is closed or not by taking the boundary on it. It showed an error that means the surface is closed. The closed surface is shown below:

Then I have just created the solid part from this closed surface using the closed surface command in part design and also i have given it a color. The solid part is shown below:

Then I have performed the draft analysis on the solid part. The draft analysis is shown below:

After creating the solid parts for the lower substrate and map pocket I have created the door armrest. For Door Armrest again I have spilt the part into two parts and named it according to me one is the door armrest cushion part and the other is the door armrest.

DOOR ARMREST:

For this again I have to first extract the class A surface from the input given. The multiple extracts are shown below:

After extracting the surface I got the class A surface but there was a gap. so I filled it with the multisection surface. The multisection surface is shown below:

Then finally I have joined the multi-section surface with the class A surface to get the final Class A surface. The final class A is shown below:

Tooling axis - For the tooling axis, I have created one point on the base surface and from that point, I have created one line along the direction in which the component is clearly visible. For the door armrest part, two tooling axis is required one is the main tooling axis and other is the slider tooling axis because the main tooling axis cannot clear the component alone.

The main and slider tooling axis is shown below:

After creating the tooling axis I have performed the draft analysis on class A. The draft analysis is shown below:

First considering the main tooling axis

In the above analysis, u can see that there is a portion that is in red which means that it has a negative draft and cannot be cleared using the main tooling axis so for clearing that portion I have used the slider axis. The draft analysis using the slider axis analysis shown below:

Now u can see that the portion is clearing now. Next, I have moved on for creating the other surfaces.

Class B surface - Again following the similar procedure that is offsetting the class A to 2.5 mm. The B surface is shown below:

Class C surface - For creating the c surface again I have used the sweep command. So I have swept the boundaries of class A along the tooling axis with a 3-degree draft. And for some parts, I have swept the boundaries using the 'with reference surface' option. The sweep parameters are shown below:

Then I have joined all the sweeps that I created to get the class C surface

Then I have joined the Class A and Class C surfaces. The join is shown below:

Then finally I have trimmed the join with the class B surface after extrapolating the B surface wherever it's required to get the final part. The final part with the closed surface is shown below:

Then I have created the solid part from this closed surface using the closed surface command in part design. The solid body is shown below: I have provided the color also to the part.

Now I have performed the draft analysis on the solid part using the slider tooling axis. The draft analysis is shown below:

Door Armrest cushion - Following the same procedure I have extracted the surfaces to get the class A surface of the door armrest cushion part. The extract is shown below:

The result that I got from these multiple extracts was Class A surface. The class A surface is shown below:

Tooling axis - The tooling axis I have taken for this component is the same as the tooling axis of the first part of the door armrest. So this also has two tooling axis one is the main tooling axis and the other is the slider axis. The two tooling axis are shown below:

Now the draft analysis is of above class-A surface is shown below:

first considering the main tooling axis:

Then considering the slider axis:

Now u can see that the surfaces which are not clearing with the main tooling axis are cleared by the slider tooling axis.

Now I have created the other surfaces that are class B and class C surfaces.

Class B surface - For the class B surface again I have offset the class A surface to 2.5 mm. The offset is shown below:

Class C surface - For creating the class C surface I have swept the boundaries along the tooling direction giving a 3 degrees draft. For some portions for creating the C surface, I have used the 'with reference surface' option to sweep the boundaries. The sweep parameters are shown below:

For some boundaries in which the sweep was a little difficult to perform so for those boundaries, I have done the multisection surface. The multisection surface is shown below:

Then I have joined the multisection and the sweeps that I created to get the class C surface. The class C surface is shown below:

Then I have trimmed the class C surface with Class B after extrapolating the class B and class C wherever it's required. The trim is shown below:

Then finally I have joined the above trim with the class A surface to get the final part. The final part is shown below

Then I have checked whether the join is a closed surface or not so for that I have taken the boundary. I got an error that proves that the surface or the join formed is a closed surface. The closed surface is shown below:

Now I have created the solid part from this closed surface using the closed surface command in part design. The solid part is shown:

Then I have performed the draft analysis on the solid part. the draft analysis is shown below:

Now I have completed the solid part creation of all 3 parts that are the lower substrate, map pocket, and door armrest. Next, I have created the flanges

FLANGES - Flanges are the elements that are needed to join different components together. So here I have to make flanges on the door armrest and the map pocket. Following the master section, given as the input basically the measurements and location of the flange. I have created the flanges. First I have created the flange on the outer map pocket. For creating the flanges I have taken extraction of the curve and made a point on that curve then created one plane on that point followed by creating a sketch on that plane taking the point created as the origin. The sketch is shown below:

Then I have padded the above sketch. The pad is shown below:

Then I have provided the draft and fillets to the flange. The fillets value can be taken from the master section master if given or u can provide a minimum fillet of 1 mm. coming to the draft value here for the outer map pocket I have provided 3 degrees and but if the flange size is less than u can provide a minimum draft of 0.5 degrees. After providing the draft and fillets the flange looks like this:

Then I have copied the flange body and paste it on the main part body using the as result with a link option in paste special.

After pasting I have translated the flange using the point-to-point translation feature keeping in mind the spacing rule that is the gap between two flanges should be 60 - 100 mm. Then after the translation, I have used the union trim boolean operation to make one single body. The outer map pocket with flange is shown below:

The same thing I did for the other parts also that is extracted the curves in which the flange is required then I made a point and plane then sketched on it to create flanges later provided drafts and fillets.

The flanges of the inner map pocket are shown below for this part I have given 0.5 degrees draft to the flanges.

The flanges of the Door Armrest are shown below for this part also the draft is 0.5 degrees:

After creating the flanges I have created the dog house.

Dog House - Dog house is an engineering feature used in the plastic trim design. Doghouses are used as supporting features. Sometimes other engineering features like snaps; locators, etc. are mounded on them to increase their strength. Dog houses are subjected to draft analysis to prevent breakage of the component during ejection from the mold cavity. Dog house and other engineering components are built on B-surface.

Here the dog house is required for lower substrate only. So for creating the dog house I have extracted the base surface of the lower substrate and made a point on that extracted surface and sketched on it. The sketch is shown below:

Then I have swept the above sketch along the tooling axis of the lower substrate giving 1.5 degrees of the draft. The sweep is shown below:

Then I have closed the surface on the top. After closing the surface I have used the thick surface command to make a solid body giving 2mm thickness. The thick surface is shown below:

now for the dog house also it will require an additional axis which is called a lifter axis that would clear the inside portion of the dog house because it won't be clear using the main tooling axis. so for creating that lifter tooling axis I have created one point on the back surface of the dog house and from that point created one line and that line is my lifter axis. The lifter axis is shown below:

Now according to this tooling axis, I have drafted the inner portion of the dog house. the draft value I have given is 0.5 degrees. Actually, I have given the draft before giving the inner fillets and that is the correct method to do it later u can give fillets. The draft is shown below:

Now for avoiding the sink mark I have followed the design rule for it which is shown below:

For this purpose, I have just offset the base of the lower substrate to a height of 4mm the value could be anything between 3 - 6 mm. and then I have extracted the inside portion of the dog house. The offset and extraction of surfaces are shown below:

Then I have extrapolated the inside portion that I extracted and trimmed it with the base which is at an offset of 4 mm. The trim is shown below:

After trimming I have the trim to 1 mm considering the design rule that it should be 40 % of the thickness of the component. The thickness of the component is 2.5 mm so 40% of 2.5 is 1mm. After offsetting it to 1mm I have split the offset surface with the dog house body. the split is shown below:

After splitting I have given one more draft The draft is shown below:

Then I have done the draft analysis on the dog house. The draft analysis considering the main tooling axis is shown below:

Here the tooling axis is my lower substrate tooling axis

Then the draft analysis considering the lifter axis is shown below:

Now we can provide the fillets. so the dog house is completed.

Next, I have created the push pins.

Push pins - Push pins are used for joining one component to another. These are basically attached to the dog house.

For creating the push pins I have taken the following reference basically the measurements.

so according to the above reference, I have created one sketch. The sketch is shown below:

now I have just inserted one body and used the shaft feature to create the solid body of the push pin. The shaft is shown below:

Then I have made the cut out on the dog house for inserting the pin. For the cut out I have made one sketch on the top surface of the dog house and extruded it. The extrude is shown below:

Then I have split the extrude from the dog house to get the cut-out. The cut out for the push pin is shown below:

Then I have just added using the boolean operation to my dog house. The dog house along with push pin is shown below:

Then I have used the copy and paste special option and translated the dog house along with a push pin to different locations on the lower substrate in which I want the dog house. so basically I have created points on the lower substrate and used the point-to-point translation. After doing the translation I have just added all the dog houses to the lower substrate. The result is shown below:

Then at last I have created the Heat stakes but let's see what is Heat staking

Heat staking - Heat staking also known as thermoplastic staking is the process of joining two dissimilar materials together. In heat staking, we use local heating and cooling to raise the temperature of plastic components and allow plastic reforming to be carried out. This reforming can be used in a wide variety of applications.

Applications range from staking plastic bosses for assembly of car door panels to joining PCBs to plastic housings. Benefits of this technique include; no vibration damage, no particulates, the ability to stake metalized coated applications, and the capability to stake in difficult to access or restricted areas.

The progressive melting of plastic under continuous pressure forms the head. When staking the right combination of heat and pressure for the application is critical.

The advantages of Heat staking are as follows:

1) simplification of the machinery

2) Reduced cost of machinery

3)Multiple fastening points

4) Allows higher density of welds compared to hot air cold form or ultrasonic welding.

Before creating the heat stakes I have created the holes on all the flanges that I created earlier. For the hole, I have created one point on the upper face of the flange and created a sketch on it. The sketch is shown below:

Then I have extruded the sketch and split it from the outer map pocket to get the hole. The extrude and hole is shown below:

Then for creating the heat stakes I have offset the extrude created to 0.5 mm because the heat stake should maintain a distance of 0.5 mm from the hole. The offset is shown below:

Then I have thickened the offset surface to get the solid body. The thickness value was 2mm and provide a draft of 0.5 mm. The thick surface is shown below:

here one thing we need to check the distance of the upper face of the heat stake from the flange surface it should be close to 7mm according to the master section given. So in my case, it was 7.018 mm which is correct.

Then I have done a similar thing for creating multiple heat stakes for the flanges and translated it using the point-to-point translation. Then at last I have used the union trim boolean operation to make it a single body. The union trim is shown below:

Now the part creation and the attachment feature creation are done.

RESULT - The draft analysis of individual part is shown below:

1) Lower substrate

2) Outer map pocket

3) Inner map pocket

4) Door Armrest

The final CAD model of the Door Trim panel is shown below:

FRONT VIEW :-

BACK VIEW :-

ISOMATRIC VIEW :-

TOP VIEW:-

The tree structure of the CAD model is shown below:

CONCLUSION - This concludes the creation of the Door Trim Panel along with engineering features using the master section given as the input and the draft analysis has also been performed on the component.