How non default directions for Solid Combine feature works | CATIA V5
Overview
In this Tech Tip, you will learn how to create solid parts where the profiles intersect at Specified Directions other than the Normal to profile direction to achieve the desired shape using Solid Combine feature.
The User Case
In the image below, solid part is created by two closed sketch profiles namely Lower_Profile and Side_Profile which are intersecting at normal direction. By default, Normal to profile direction is selected in Combine Definition dialog box and then further we have to select Lower_Profile sketch and Side_Profile sketch in the First component and Second component sections respectively from the Combine Definition dialog box.
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Figure: Selection of Lower_Profile sketch and Side_Profile sketch with Normal to profile as the default direction
Now we need to create solid part using Solid Combine feature with some specific directions other than the Normal to profile direction.
Please follow below steps and video to achieve the required result –
Case 1
Creating a Solid Combine feature using Normal to profile direction for Side_Profile sketch and other specific direction for Lower_Profile sketch.
Step 1:
Open Solid_combine.CATPart
Step 2:
Select Sketch-Based Features | Solid Combine
CATIA displays the Combine Definition dialog box and prompts you to pick the first profile –
Step 3:
In the Specification Tree, select Lower_Profile sketch for the First component section from Combine Definition dialog box. Alternatively, you can pick the sketch labeled 1 from the Graphics Window –
Step 4:
In the Specification Tree, select Side_Profile sketch for the Second component section from Combine Definition dialog box. Alternatively, you can pick the sketch labeled 2 from the Graphics Window –
Step 5:
Right click on the Geometrical Set named as Direction Lines and select Hide/Show option in contextual menu.
Step 6:
From the Combine Definition dialog box, for the First component section, unpick or deselect the Normal to profile option and select the line named as Lower Profile Direction from the Specification Tree –
Figure: Preview of combined solid with one profile extruded in normal direction and other profile extruded in a direction other than normal direction
Step 7:
In the Combine Definition dialog, click OK to create the combined solid.
CASE 2
Creating a Solid Combine feature using Normal to profile direction for Lower_Profile sketch and other specific direction for Side_Profile sketch.
Repeat steps 1 & 2 from case 1 or refer below steps.
Step 1:
Open Solid_combine.CATPart.
Step 2:
Select Sketch-Based Features | Solid Combine.
CATIA displays the Combine Definition dialog box and prompts you to pick the first profile.
Step 3:
In the Specification Tree,
Select Lower_Profile sketch for the First component section from Combine Definition dialog box.
Alternatively, you can pick the sketch labeled 1 from the Graphics Window –
Step 4:
In the Specification Tree,
select Side_Profile sketch for the Second component section from Combine Definition dialog box.
Alternatively, you can pick the sketch labeled 2 from the Graphics Window –
Step 5:
Right click on the Geometrical Set named as Direction Lines and select Hide/Show option in contextual menu.
Step 6:
From the Combine Definition dialog box, for the Second component section, unpick or deselect the Normal to profile option and select the line named as Side Profile Direction from the Specification Tree –
Figure: Preview of combined solid with one profile extruded in normal direction and other profile extruded in a direction other than normal direction
Step 7:
In the Combine Definition dialog, click OK to create the combined solid.
Case 3
Creating a Solid Combine Feature using specified direction Lines Lower profile Direction and Side profile Direction other than Normal to profile
Repeat steps 1&2, again.
Step 1:
Open Solid_combine.CATPart.
Step 2:
Select Sketch-Based Features | Solid Combine.
CATIA displays the Combine Definition dialog and prompts you to pick the first profile.
Step 3:
In the Specification Tree,
select Lower_Profile sketch for the First component section from Combine Definition dialog box.
Alternatively, you can pick the sketch labeled 1 from the Graphics Window –
Step 4:
In the Specification Tree,
select Side_Profile sketch for the Second component section from Combine Definition dialog box.
Alternatively, you can pick the sketch labeled 2 from the Graphics Window –
Step 5:
Right click on the Geometrical Set named as Direction Lines and select Hide/Show option in contextual menu.
Step 6:
From the Combine Definition dialog box, Unpick or Deselect the Normal to profile option for both the Component and Select the Lower Profile Direction, Side Profile Direction for the First and Second component Direction respectively from the Specification Tree –
Figure: Preview of combined solid with both the profiles extruded in specified direction other than normal direction
Step 7:
In the Combine Definition dialog, click OK to create the combined solid.
Case 4
Changing Angle values of the specified direction lines named as lower profile Direction and Side Profile Direction
Step 1:
Double click on the line named as Lower Profile Direction from the Specification Tree, CATIA displays Line Definition dialog box.
Step 2:
Change the Angle value of line Lower profile Direction to 300deg and
click OK in the Line Definition dialog box
Step 3:
In the Line Definition dialog, click OK to create the Solid combine.
Step 4:
Double click on the line named as Side Profile Direction from the Specification Tree, CATIA displays Line Definition dialog box.
Step 5:
Change the Angle value of line Side Profile Direction to 325deg and click OK in the Line Definition dialog box
Step 6:
In the Line Definition dialog, click OK to create the Solid Combine.
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