Week 9 - Attachment Feature Creation - Challenge 2

Objective: To create surface B and surface C with thickness of 2.5mm with considerable draft angle for the given Class A Surface and to create engineering features of dog houses with their standards in mind.

Part I - Closed Surface from Class A Surface:

Material suggestion:

Polybutylene terepthalate (PBT):

good chemical resi9stance and bearing and wear properties.

Acrylonitrile Butadiene Styrene (ABS):

good balance of impact, heat, chemical and abrasion resistance, dimensional stablity, tensile strength, surface hardness, rigidity and electrical characteristics.

Tooling Axis:

Core and Cavity Tooling axis:

When a plastic body is created in a molding, the core is moved with respect to the cavity in a linear path. The joining line of core and cavity is called the tooling axis, The plastic component is poured and ejected respectively to hat axis of the core and cavity motion.For, this above challenge to be satisified, the discussed tooling axis must be created for the product, keeping the motion of core and cavity in mind.

Slider Tooling axis:

Here the slider tooling axis is used to show the motion of the slider to create the dog houses.

Steps in Catia to add tooling axis:

1. An visual analysis by us to be undertaken at every axis plane of X, Y and Z to come up with the suitable plane that holds majority of the features of the Surface A.
2. Here the X and Z axis, doesn't suit the above requirement, hence moving to Y plane, we are able to preserve majority of the details provided in Class A Surface.
3. At First we must create a geomentrical set, where it should be renamed as "Tooling Axis"
4. To Fix Y axis as the tooling axis, we must construct line on the Y-axis to represent it.
5. For the line creation, we can use the hole present in the surface A as the reference and using the point option, we must extend it on the both sides for a considerable distance with Y-axuis direction.
6. Now to comfortably view the final tooling axis, we must publish it separetly using publish command in the tools option, this saves the time to search the geomentrical set in a long feature tree.

Tooling axis snippet:

Slider Tooling axis snippet:

Class A Surface:

• Starting with the Class A as the input, and required output as the plastic component, we should consider the following:
• The Surface A is the asthetic part of the given component. Hence, changes made over Class A Surface should be avoided.
• Draft Angle must be on the Class C Surface.

Steps in Catia to import Class A Surface as neutral file (STP, IGS):

1. Using open option in the catia file menu, the class A Surface file is opened from either IGS, STP or CatPart.
2. If it is in IGS format, the surface A must be joined using distance propagation.

Class A Surface snippet:

Draft Analysis:

When the final componet is created, the drafting analysis done to ensure the draft angles are given to the surface C is within the standard range of 3 degree and 90 degree. By giving this angle, the plastic component is protected from damage while it is ejected. The colour order of GBR in the order of Green, Blue or Red.

• if the draft shows green colour, then the draft angle is clearing the 3 degree angle.
• If the blue colour is highlighted, then the draft is somewhere between 0 and 3. This area must be studied to make its value close to the 3 degree clearance.
• if the red colour is highlighted, then the draft is below 0 degree, this colour seperates the core from the cavity or slider.

Draft Analysis to the engineering feature, must also be checked.

Here, the dog house is the only feature that is made, so the outer draft of 1.5 degree and inner draft of 0.5 degree, should also be studied by changing the green value and the tooling axis with slider axis at necessary positions respectively.

Steps in Catia to Drafting Analysis:

1. Add material using the view option to let the draft analysis to run.
2. Select the surface or final part body to make it highlighted in the feature tree.
3. Use the analysis in the insert option in the CATIA's menu bar, to find the Feature draft analysis.
4. Now after selecting the option, two pop window will be displayed, where:
5. One has the colour coding, where we must define the colors in the order of GBR (Green, Blue, Red) respectively and set the angle value to be 2.9 for Green, 0 for Blue, and less than 0 as Red.
6. Other pop up has several tools for draft analysis, Now from the right most corner of the screen, drag the direction compass and place it on the tooling axis, where the resulting compass aligns with the tooling axis. Now after it gets aligns, lock the compass position using Compass Lock tool.
7. To view the draft analysis, select the Surface or final closed body. By choosing it as mentioned, the analysis produces the color coding over the parts where the draft condition/angle satisfies as we mentioned.

1. Draft Analysis - Class A Surface:

2. Draft Analysis - Closed Body clearing by Class A Side:

3. Drafting Analysis - Closed Body with Engineering Features clearing by tooling axis:

4. Drafting Analysis - Closed Body with Engineering features clearing by slider axis: 

Class B Surface:

The Class B surface is the other side of Class A surface of the plastic component and where the portion sits on the core.

Make Class B as the sacrificing portion of the component at the core, we ensure the ejector pins motion to push the finished component out of the mold to fall on Class B, again saving Class A from the stress from ejector pins.

Steps in Catia to Create Class B Surface:

1. Study the Class A surface features by using vernier measure tool to distinguish between the flat and curved surface, by the symbol appears next to it.
2. Extract the flat ones by using extract command and leaving behind the curved unelected.
3. Now offset the extracts by using the thickness value 2.5 as the offset and now use the untrim command to derive the untrimmed surfaces from the offset.
4. Due to the lack of intersection, we must use extrapolate tool by point continuity to make them intersect with each others respectively.
5. Now trim the required parts and save in separate geometric sketch.
6. Give the fillets to the intersecting corners as per the Surface A but, following the Fillet offset rule, where the bulging upward fillets value must be reduced by thickness and vice versa for the building downward fillet.
7. Now the Class B surface is created successfully.

Class B Surface snippet:

Class C Surface:

• The Class C surface is the in between portion of Class A and Class B, where the volume is added or in other words, plastic thickness is given here. 
• The Class C Surface is given the draft angle of 3.
• To make the component to be easily ejected from the mold, it requires 3 degree draft angle.

Steps in Catia to create Class C Surface:

1. Use the Class A surface as the reference and extract the boundaries individually on every sides where the curvature changes using boundary tool with tangent continuity. 
2. Now use the "swept tool" and "with draft directions" to extrude the boundaries and tooling axis as the guidelines and with draft angle as 3 degrees in outward direction.
3. Now use the extrapolate tool to intersect the swept extrudes by selecting the unintersected edges of the swept extrudes to intersect with adjacent swept extrudes.
4. Use the trim to join the swept surfaces.
5. Save it in a separate geometrical set.

Class C Surface Snippet:

Final Trim:

• The resulting surface being formed after joining the Class A, B and C as per the above spoken features specific to the surfaces respectively is done in Final trim.
• This showcases the cavity's and core's design of how the mold should be created.

Steps in Catia to create joined Class A, B and C Surface (closed):

1. Use the join command to join the Class C surfaces of boundary and hole swept extrudes with Class A.
2. Use the trim command to trim the extended edges of the class C with Class B.

Final Trim Snippet:

Solid Body:

Solid body is the part body created after calling the closed surface command on the Final trim surface.

Steps in Catia to create Closed part body:

1. Use the closed body tool in part design to create the part body.
2. Run Draft analysis using feature draft analysis from tools, and selecting the part.

Solid Body snippet from Class A Side:

Solid Body snippet from Class B Side:

Part - II: Engineering Features - Dog House:

Explanation: Dog House is a supportive feature that is used to hold screw bosses, snap fits or locators, where the mentioned features required a vertical clearance to combine with another plastic material.

Design consideration of the Dog House:

1. The Height of the Dog house must not exceed 60mm.
2. The wall thickness of the Dog house must be within the range of 2.5mm.
3. Draft angle of the exterior walls must be given 1.5 degree.
4. Draft angle of the interior walls must be given 0.5 degree.
5. The fillets provided should be more than 0.5mm.
6. Width of dog undercut area must be = 3W.
7. Height of the undercut should be between 3-6mm.

Dog House Design snippet:

Sketch Status:

Four views of Dog House:

End of Report.