In this step, you will transfer a Cam to SolidWorks.
1.Open a Part or add a new Part in SOLIDWORKS.
2.Use the Cam-Coordinates dialog-box to send the Cam to SolidWorks from MechDesigner.
If the Cam-Coordinates dialog-box is not open:
STEP 1: Double-click the Cam-Data FB in the graphic-area
If the Cam-Coordinates dialog is not linked to a Cam, then:
STEP 2: Click a 2D-Cam in the graphic area or Assembly-Tree.
STEP 3: Click the Traffic-Light icon
When you click the Traffic-Light in this dialog-box, MechDesigner calculates the Cam-Coordinates with the active settings. Experiment with the icons to understand the icons.
You can calculate the cam using:
•Biarcs in which you define the maximum allowable chord error - the cam is transferred to SolidWorks as Arc sketch-elements.
•Equal Increment of Machine Angle - you define the number of points - the cam is transferred to SolidWorks as a point to create a Curve feature. which will then be defined as a Spline when you 'convert-entities'.
There are some limitations with the Curve feature:
•The Curve (Cam) cannot cross at any place, or 'self-interfere'.
•If there is a 'step-in-velocity' (or position), then it is possible there will be a 'kink' in the Spline.
•YOU must be careful to make sure the Motion from which the cam is derived (in MotionDesigner) is continuous in at least Position and Velocity.
•You would usually want it be continuous in Acceleration also. Continuous Acceleration is very important when the cams drive machines.
See Cam-Coordinates dialog-box for more details. EXPERIMENT.
2.Open a Part, or add a new Part and save it.
4.Arrange MechDesigner and SolidWorks so that you can see the two applications.
Make sure only ONE SolidWorks application is running.
In the Cam-Coordinates dialog-box (in MechDesigner again)
1.Click 'Send to CAD', (the SolidWorks icon next to the Rebuild button)
I find that if I click the SolidWorks application, then the Cam shows more quickly.
MechDesigner draws three 'Curves' on the Front Plane of the SolidWorks Part. The three curves features are:
•2D-Cam-Data (which is the Cam1 or Cam 2 (external or internal)
•X-axis : Two Point in the curve, 0,0 and 100,0
•Y-axis : Two Point in the curve, 0,0 and 50,0
If required: to send the 'other' Cam:
2.Click the 'other cam' in the Cam-Coordinates dialog-box and 'Send to CAD' again.
3.Do again for the Pitch-Circle, if required.
In SolidWorks, for example, if you want to make a 2D-Groove or Track Cam:
1.Start a sketch on the Front-Plane.
2.Add a Circle. Make its diameter greater than the radius of the larger Cam.
3.Use Insert > Base/Boss > Extrude to extrude the circle to the full thickness of the Cam part.
4.Add a sketch to the face of the Cam.
5.Click a 2D-Cam Curve feature
6.Use Tools > Sketch Tools > Convert Entities.
7.Do 1-3 again for the other 2D-Cam.
8.Use Insert > Cut > Extrude. to extrude a cam groove into the Cam blank.
9.Cut a Hole through the center for a Shaft, key-way, etc.
SOLIDWORKS Export Options interface.
In SolidWorks, to save the file as a STEP file ready for a CAM program, you must make sure the 'Export 3D Curve features' check-box is checked.
1.Click File > Save as... and enter a file-name for the cam
In the 'Save as type:' drop-down box,
3.Click STEP AP203 file type
4.Add a description
5.Click the Options button, at the bottom of the File > Save as... dialog
In the Export Options dialog
5.Make sure the 'Export 3D Curve features' check-box is checked - see left image
6.Click the OK button to close the Export Options dialog
7.Click OK button to save the cam as a STEP file.