Let’s Design Control Arm With Solidworks – Solidworks Tutorial

174
Design Control Arm With Solidworks

Mastering one of design software is a must for current design engineers. It’s even better to master more than one of software design. Because in general the company will find employees as engineers who master software design such as Autocad, Mechanical desktop, Autodesk Inventor, Solidworks, Catia, Pro-e and others. Therefore, if we have aspirations to become an engineer, we must master one of these software. Here I will try to show how to design control arm with Solidworks, which I have previously tried to design control arm with Autocad.

Design Control Arm With Solidworks – Solidworks Tutorial

– First, open Solidworks, then click File, then select New or control N, and select Part.

– Select Sketch Menu and then click sketch

– Click Top Plane

Design Control Arm With Solidworks,

– Select circle menu, click center axis in area drawing and move a bit and click 1 time. Select line menu, click center axis in area drawing and move cursor so that make horizontal line and click again (we don’t give size to line or circle cos if we use solidworks, we will give the size after we make circle or line, different with autocad method. Check the video tutorial below to know more about this)

– Click circle again and click the end of line that have just made and move a bit until you make circle.

Design Control Arm With Solidworks,

– Then we make a slash upward, click line menu, click center second circle and slide the cursor up so that it looks like this,

Design Control Arm With Solidworks,

– Click line menu and then click the end of second line, move a bit until we make circle.

Design Control Arm With Solidworks,

NEXT STEP

– We will give size or dimension to all of object. Click smart dimension menu, and click first circle and move to outside circle and click 2 times and type the dimension 60 mm (diameter) then enter.

Solidworks tutorial

– Give dimension to other object again. Click smart dimension and select first line and move a bit then click 2 times, type the size is 100 mm.

Solidworks tutorial

– Next, please give dimension to all of object. Second circle, the diameter is 100 mm. Third circle, the diameter 50 mm, and the size of second line is 125 mm and then the angle is 129. To give dimension of angle, the first you select smart dimension menu then click second line then click first line and move the cursor up and click 2 times, type 129 and click the green check or enter.

Design Control Arm With Solidworks,

– Now we will use Arc menu. Click arc menu choose arc with 3 point, select first circle and select second circle and move outside circle and enter.

Design Control Arm With Solidworks,

– Give dimension to arc object, the radius is 40 mm. Select smart dimension, click arc and move up then click 2 times, type 40 then enter. Still using smart dimension, click arc then click first circle and click arc, move cursor up, click 2 times, type the size is 34 then enter. Select arc again then select first circle and move cursor left and type 2 times, type 61.15 then enter.

Tutorial of CAD

– Next, mirror the arc with mirror about the line that the size 100 mm. Select mirror menu, click the arc then click the line and enter or check the green check.

Tutorial of CAD

– Make arc again. Click arc menu choose arc with 3 point, select second circle and select third circle and move up a bit then enter.

Design Control Arm With Solidworks

Continue to Design Control Arm With Solidworks – Solidworks Tutorial

– Now we will give dimension to arc object. Select smart dimension, click arc and move up then click 2 times, type 60 and enter. Still using smart dimension, click arc then click second circle and click beginning of arc line and move right, click 2 times, type the size is 7.25 then enter. Select arc again then select end of arc line and move cursor down and type 2 times, type 10 then enter. (Make all lines black, it means locked and you can not move the line or arc)

Design Control Arm With Solidworks

– Next, we will mirror the arc that we have just made. Select mirror menu, click the arc then click center line of second circle and third circle that will use to be mirror about.

Design Control Arm With Solidworks

– Now we will trim all lines and arc that’s not used. Select trim and click all lines and arc that you want.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Next step, we will extrude the sketch. Select FEATURES => EXTRUDED BOSS/BASE

Design Control Arm With Solidworks

– Fill all of parameters for extruded. Choose Mid Plane cos we want to extrude 2 directions (up and down), type the size is 50 mm, select the object in area drawing and enter.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Then select Sketch menu and click top area object.

Tutorial of CAD

– Click top view

Tutorial of CAD

– Make arc and circle that follow all circles and arc that have just extruded.

Tutorial of CAD

– And trim all arcs that’s not used. See the result is like below:

Solidworks Tutorial

– Select Isometric view, select Features – Extruded Cut. Select the area that we will extruded cut, type the size 5 mm, and make sure the arrow is downward in area drawing.

Solidworks Tutorial

Continue to Design Control Arm With Solidworks – Solidworks Tutorial

– Now we will extrude cut again but we will use mirror part. But before we extruded cut, we have to show the TOP PLANE this part. See the picture below:

Solidworks Tutorial

– Next, select cut extruded that have just made and click mirror part.

Solidworks Tutorial

– Select top plane then enter or click green check.

Solidworks Tutorial

– Next step, we will make hole using Hole Wizard. Select hole wizard, and fill the parameters.

Solidworks Tutorial

– In the positions menu, click top area of first circle. Give dimension with select smart dimension, then select first circle then click center of hole.

Design Control Arm With Solidworks

– Move a bit and fill the size is 0. And give the dimension to other side with size 0 then enter or check the green check 2 times.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Make hole again in third circle. Select hole wizard, fill the parameters below:

Design Control Arm With Solidworks

– Select positions to place the hole and make dimension. Give the dimension 0 to X and Y.

Tutorial of CAD

Tutorial of CAD

– Click Zoom to Fit menu then select sketch menu, click top of second circle. Active Top view.

Design Control Arm With SolidworksDesign Control Arm With Solidworks– Select zoom to area menu then zoom second circle / big circle.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Select circle menu and then click center second circle and move a bit and enter again.

Design Control Arm With Solidworks

– Give dimension, select smart dimension, click the circle and move right or left the cursor and click 2 times, type the dimension is 80 and enter.

– Make line from center point of circle, select line menu and then click center circle then move right and click again. Give dimension 20 mm.

Design Control Arm With Solidworks

Next of Design Control Arm With Solidworks – Solidworks Tutorial

– Make circle again with center point is the end of line that have just made. And give the dimension 50 mm (diameter)

Design Control Arm With Solidworks

– Make line from center point of second circle or big circle to left quadrant. See the picture below.

Design Control Arm With Solidworks

– Now we will use offset menu to offset the line that we have just made. Select offset entities menu, click the line, fill the dimension 6 and enter or check the green check.

Design Control Arm With Solidworks

– Trim all lines that’ not used. Select trim entities, then select trim to closest, then click the line that you want to trim.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Delete all line that is not used until like below:

Design Control Arm With Solidworks

Next of Design Control Arm With Solidworks – Solidworks Tutorial

– Give dimension the object with smart dimension.

Design Control Arm With Solidworks

– Click zoom to area, zoom the cone. Select arc menu and make arc. See the picture below:

Design Control Arm With Solidworks

– Give dimension the arc with radius 5 mm.

Design Control Arm With Solidworks

– Trim all lines that is not used until like below:

Design Control Arm With Solidworks

– Now we will extruded cut with the sketch that have just made. Before you begin to extruded cut, click isometric view first. Select extruded cut menu, choose through all, select the sketch then enter.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Show the front plane, cos we will mirror the extruded cut. After that select cut-extrude2 in feature manager, then click mirror menu.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Select the front plane and then enter or check the green check.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Hide front plane. Now we will make hole in the second circle. Select hole wizard menu, and fill the parameters,

Design Control Arm With Solidworks

– Select positions menu then click top of second circle, and give dimension 0 cos we want to place the circle in the center of circle radius 25 mm, then enter. Check the picture below:

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Mirror the hole 3 mm with top plane as mirror face. Select hole 3 in feature manager, then click mirror, and select top plane then enter.

Design Control Arm With Solidworks

Design Control Arm With Solidworks

– Click top view and hide top plane. Make hole gain, with diameter 8 mm and through all. follow this picture.

Design Control Arm With Solidworks

– Select positions menu, and then click top of circle radius 22 mm.

Design Control Arm With Solidworks

– Select smart dimension and give dimension and then enter, see the picture:

Design Control Arm With Solidworks

– Now we will use circular pattern to copy the hole become 6 hole. Select Hole4 in feature manager, choose circular pattern,

Tutorial of CAD

– Fill the parameters, click the circle diameter 44 mm then enter, see the picture below:

Tutorial of CAD

Tutorial of CAD

Tutorial of CAD

Tutorial of CAD

– For finishing, you can do chamfer to the angle side that need it. Select chamfer then fill the parameters and choose the line or angle side.

Tutorial of CAD

– If you want to give material to this part you can select Appearances menu, select metal that you want.

Tutorial of CAD

Tutorial of CAD

That’s all and thanks for coming to my blog. Please share this article and follow my fans page facebook so that you can get the updated tutorial from me. And if you are still confused about this tutorial please come to my video tutorial in Youtube, also don’t forget subscribe my Youtube Channel.

LEAVE A REPLY

Please enter your comment!
Please enter your name here