Week 9 - Project - A pillar Design with Master Section

A_PILLAR_MASTERSECTION

First of all I got the class a surface and master sections then I created b surface, c surface, close body, and b side features in several parts.

At first I created two geometry sets and named it as master section and class a after I put the class a surface in to class a geometry and master sections in master section geometry.

TOOLING AXIS – I extract a surface from class a by using extract command after I created a point using surface method and then I created a line using point-direction method for point pick the point 1 and for direction pick the y component. After creating line I named it as tooling line.

DRAFT ANALYSIS 1 – For checking of my tooling line was proper or not I create draft analysis of class a. For draft analysis I took the feature draft analysis command and pick the compass on tooling line and pick the class a surface, I gave the draft angle 2.9degree and then I saw that class a turned in to green colour and when I changed draft direction then it turned into blue colour that`s mean my tooling axis is correct.

CLASS B – For class b I offset the class a by 2.5mm which was the thickness of component. After offsetting I saw that there were a surface vanished by offsetting so I created it by using sweep command. For sweep operation I insert a plane for reference I gave YZ plane and for point I pick vertex 1 of offset and got a plane. After that I insert the two boundaries by tangent continuity from offset1. After that I took the sweep and explicit command, sub type as with reference surface for guide curve pick the boundary 1 and for profile pick the boundary 1 and draft value gave zero then I got the surface. After that I join the sweep surface with offset. After that I extrapolate the join 1 with curvature continuity and for propagation mode I gave point continuity and for length gave2.25mm. After that I named it as b surface.

CLASS C – For class c surface I insert boundary from vertical edge of class a and took the sweep and line command, sub type as with reference surface for guide curve pick the boundary 3 and for reference surface pick the class a and draft value gave 93degree then I got the surface. After that I insert new boundary from second vertical edge of class a and took the sweep and line command, sub type as with reference surface for guide curve pick the boundary 4 and for reference surface pick the class a and draft value gave 93degree. After that I insert boundary from horizontal edge of class a and took the sweep command, sub type as with reference surface for guide curve pick the boundary 5 and for reference surface pick the class a and draft value gave 90degree then I got the surface. After that I insert new boundary in two parts from horizontal edge of class a and took the sweep command, sub type as with reference surface for guide curve pick the boundary 6 and for reference surface pick the class a and draft value gave 90degree then I got the surface. After that I took the sweep operation subtype as with reference surface, guide curve as boundary 7, for reference pick the class a and draft angle gave 90degree. After that I saw that there were some gap on sweep 5 and sweep 6 so I created a point on edge of sweep 6 and created a line using point to point method after that I split the sweep 6 by cutting element as line 2. After that I created two lines using point to point method and for point pick the close edge of sweep 5 and split. After that I took the multi section command and for section pick the boundary8 and 9 for guide pick the line3 and 4 then fill the surface. After that I join the multi section1, sweep5 and split1. After that I extrapolate the sweep2 edge  with curvature continuity by 3mm and then extrapolate edge of extrapolate2 by 3mm with curvature continuity. After that I extrapolate the sweep3 edge with curvature continuity by 3mm and then extrapolate the edge of extrapolate4. After that I extrapolate the edge of sweep4 with curvature continuity by 3mm and then extrapolate the edge of extrapolate6 with curvature continuity by 3mm. After that I extrapolate the edge of join2 with curvature continuity by 3mm and the extrapolate the edge of extrapolate8 with curvature continuity by 3mm.At last I trimmed the extrapolate3, extrapolate5, extrapolate7 and extrapolate9 and named it as c surface.

CLOSE SURFACE – In this step I trim the class a with c surface. After that I trimmed the trim2 with b surface and I got the close surface.

CLOSE BODY – For close body I insert a body and went to part design workbench and took the close surface command and pick the trim3.

B SIDE FEATURES – For b side features I created it in to two parts:-

1 – DOG HOUSE OUTER SURFACE

2 – DOG HOUSE INNER SURAFCE

1 –– DOG HOUSE OUTER SURFACE - For outer surface of dog house I extract an edge from curve3 and create the point on middle of extract. After that I insert a plane from curve 3 and then create another plane on point 3 and for reference plane gave plane2. After that I create a position sketch using plane3 and for projection point pick the point 3. After that I extrude it beyond the master section.

After that I insert a plane from curve 2 and then I insert a new plane from plane4 and for point pick the point3. After that I created a new positioned sketch using plane5 and for projection point pick the point 3. After that I extrude it beyond my first extrude and extrapolate it with curvature continuity by 10mm for propagation mode gave point continuity. After that I offset it by 27mm from master section I measure the distance. After that I trim the extrude 1 with extrapolate10.After that I insert a new body and named it as dog house outer body and went to part workbench and took the thick surface command and pick the trim4, pick the arrow outside and gave the offset value 2mm witch the thickness of dog house from master section. After that I gave the fillets, for outer surface gave 3mm which is the nominal fillet value plus thickness of dog house. For inner fillet gave 1mm which is the nominal fillet value.

DOG HOUSE INNER SURFACE – I completed dog house inner surface in three step.

1 RIBS – For ribs I created a positioned sketch for reference pick the plane3 and for origin gave the projection point and pick the point 3.

After that I extract the sketch8 in three part and extrude them one by one. After that I insert a body and named it as ribs. After that I went to part design workbench and took the thick surface command and thick the extrude3, extrude4, extrude5 one by one. After that I split the thick surfaces from offset2.

C AREA – For c area I extracted the all four surface of trim4. After that I offset the extract7 by 1mm. After that I offset the extrat6 by 1mm. After that I offset the extract9 by 20.5mm. After that I extrapolate extract8 with curvature continuity by 10mm and for propagation mode gave the point continuity. After that I extrapolate the offset3 with curvature continuity by 10mm and for propagation mode gave the point continuity. After that I extrapolate the offset 4 with curvature continuity by 10mm and for propagation mode gave the point continuity. After that I extrapolate the offset5 with curvature continuity by 10mm and for propagation mode gave the point continuity. After that I trimmed the extrapolate11, extrapolate 12, extrapolate13 and extrapolate14. After that I went to part design workbench and define the dog house outer body and split the trim5.

KEY HOLE – For key hole I insert a plane using through two line for line1 pick the curve3 and for line 2 pick the curve2. After that I created position sketch using the plane6 and point3. After that I insert a new body and named it as key hole. After that I went to part design workbench and pad the sketch9.

DOG HOUSE ASSEMBLY – In this step I insert a new body and named it as dog house assembly. After that I assembled the dog house outer body and then I done union trim of ribs, for union trim I the inner rib surface for face to keep. After that I remove the key hole body from dog house assembly.

PART BODY – To create all body together I define in to part body and add the close body then I union trim the dog house assembly for face to keep I pick the upper face of dog house near from key hole.

DRAFT ANALYSIS 2 – For second draft analysis I pick part bod in material mode and took the feature draft analysis and pick the compass on tolling line and pick the part body and gave draft value 1.45degree then I saw that all surface of dog house and close body clearing the tooling line but there were small surface of class c and dog house not cleared.