TheCNC2020 - Designing the Base Support on TopSolid'design 7 #2
TopSolid 7 is a revolutionary product to meet the needs of manufacturing companies, big and small.
TopSolid 7 software includes many modules. This article will cover TopSolid'Design.
To better understand TopSolid'Design, let's learn some basic commands in Designing the Base Support to design a simple part.
In lesson 1, we became familiar with the TopSolid 7 Software interface and learned: Creating the first sketch, Extruding the solid model, Creating a rectangle.
In this article, we will continue to study TopSolid'Design, including:
- Creating a pocket
- Creating a contour
- Trimming by profile
- Adding another rectangle for trimming
- Creating a new sketch and adding a pocket operation
- Adding some fillets
- Dragging and dropping a fillet
- Using the contextual menu to add a fillet
- Editing an operation
- Creating a pattern union
Creating a pocket
- Select the Fillet command from the 2D Sketch tab.
- Adjust the radius value to 5mm.
- Click on the lower right corner of the sketch to apply the fillet.
- Close the Fillet dialog box by clicking on the icon.
- Click on the yellow arrowhead and move it up and down so that the pocket is 6mm deep, and then click on to confirm the operation. You can also double-click on the label next to the arrow to change its value.
Creating a contour
- Right-click on the face shown opposite.
- Select the Sketch command.
Note: The Contour command was launched automatically, that is the tool we are going to use in the next step.
- Create the contour by selecting the points shown below, in the order specified.
- Select the point shown below to swing a 180-degree tangent arc.
- Place the cursor directly under the first point (as shown by point 4 below). By doing this, a dynamic reference should appear. Left-click to position the point and dynamically add the relation.
- Select the Tangent arc mode again and select the top horizontal line to close the sketch as shown below.
- Click on to confirm the contour.
- Select the center point of the circle arc to the left and drag your mouse up and down without releasing the left mouse button. This shows the automatic constraints in action.
- Select the same point and drag it down to the bottom edge of the model and hover a second before you release the left mouse button. If done correctly, you will create an automatic coincident constraint between the center point of the circle arc and the edge of the model as shown below.
- Follow the same procedure to create the second coincident constraint between the other center point of the circle arc and the edge of the model.
- Add the following three dimensional constraints.
- Close the Constraint dialog box by clicking on the icon.
Trimming by profile
- Make sure the trimming arrow is pointing towards the inside of the sketch, and then click on to confirm the trimming operation.
Note: If the sketch is still shown on the screen after the operation has been confirmed, you can hide it by doing one of the following:
1) From the graphics area, right-click on the sketch and select the Hide command.
2) From the Entities tree, open the Sketches folder and uncheck the box in front of the sketch you want to hide.
Note:
+ If the Entities tree is closed, click on the TopSolid 7 icon at the top left of the screen and then select View > Entities to open the tree. The Entities tree appears on the left or right of the screen.
+ If the Entities tree is hidden, click on the corresponding tab on the left or right of the screen and then click on the icon to pin the tree.
Adding another rectangle for trimming
- Right-click on the face shown below and create a new sketch on it.
- Draw the following rectangle and constrain it as shown below and then close the dialog box.
- Right-click in the graphics area and select the Trim by Profile command.
- Make sure that the trimming arrow is pointing toward the inside of the sketch, and then click on to confirm the operation.
Creating a new sketch and adding a pocket operation
- Right-click on the face shown opposite to create a
new sketch on it.
- Draw the following rectangle and constrain it as shown in the image below.
- Select the planar face of the model as shown below, and then click on to confirm the operation.
- The depth of the pocket will therefore always be limited to the location of that specific face.
Adding some fillets
- Go to the Shape tab and select the Fillet command.
- Enter the radius value of the fillet as 6mm.
- Open the Edges dialog box and then select the three edges shown on the model below.
- Click on to confirm the fillets.
Dragging and dropping a fillet
To use drag and drop, hold down the Ctrl button on your keyboard, and with the left mouse, select the element of the model that you want to copy and paste in a new area. In this case, you will drag the 6mm fillet that you added in the previous step and drop it onto the vertical edge located above the fillet.
- Hold down the Ctrl key and then click on the fillet shown opposite .
- While still holding down the Ctrl key, drag and drop the fillet on the edge shown opposite .
- After selecting the edge, release the mouse button.
Note: You might need to use "rotary picking". To do this, just put the mouse cursor near the element that you want to select. Then click and hold down your left mouse button. Now while you are holding down the left mouse button, start tapping your right mouse button. Keep tapping the right mouse button until the edge or face that you are trying to select is highlighted. Then, release the left mouse button.
Using the contextual menu to add a fillet
Right-click on the edge shown below, select the Fillet command from the contextual menu, and then add a 5mm fillet to the edge of the model.
Editing an operation
- Double-click on the face of the fillet that you just added. This will bring up the driving dimension (radius value).
- Double-click on the dimension and adjust it to 3mm.
- Double-click on the fillet face again to hide the driving dimension.
- Right-click on the face of the 3mm fillet that you created in the previous step and select the Edit command.
- Select the edge shown below to add it to the definition of this fillet. Once selected, click on to confirm the fillet.
Creating a pattern union
In the previous commands, we have already designed half of the object. In the following step, you will learn how to mirror what is already designed.
The steps are as follows:
- Go to the Shape tab and select the Pattern Union command.
- Click on the icon to the right of the Pattern field in the dialog box.
- Select Symmetrical Pattern from the drop-down menu.
Note: You need to create a new template. You can dynamically create a new pattern within the Pattern Union command itself. Moreover, you can reuse the created pattern at a later date by selecting it directly from the drop-down list if needed.
- From the drop-down menu, select Plane as the symmetry type.
- Select the planar face shown below as your symmetry plane and select Symmetry as the transform type.
- Click on to confirm the symmetrical pattern.
- Click on to confirm the pattern union.
And this is the result after taking the symmetry.
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