Hi guys! I gotta say that I'm really new into product design and some of mechanical engineering, I'm actually an electrical engineers, but for earning my monthly wage I had to recycle myself :-)
Well, I come from plain AutoCAD 2014, on which I used to do 3D modeling and then section snapshots for drawing annotations. This way works, but I find is very time consuming and specially if you wanna make changes. That's why I decided to try SolidWorks which I'm sure I'll find easier. (I'm actually learning it)
I gotta model this tap, and I having problems figuring out how to model "that" transition between staight side and cilindrical base. I have thought on a Loft using several splines as guide curves, but I'm just not shure if the thing will work out.
Since i have no expertise, before frustrating myself in countless atemps, I'd like to have some advice from experts. So all the help is appreciated.
See attached solidworks 2014 file which matchs the rendering for modeling and blending techniques
Answered with a tutorial: https://grabcad.com/tutorials/approach-to-model-this-tap-in-solidworks-2012--1
AttachmentsSolidworks 2014 Shape Blending Faucet Example.SLDPRT, 363 KB
How about this?
Answered with a tutorial: https://grabcad.com/tutorials/approach-to-model-this-tap-in-solidworks-2012
Attachmentszzz.stp, 110 KB
I cannot model it for you as I am doing a repair install of my software at the moment, but I have some suggestions.
1. Create the sketch as shown in step2 above on the front plane and as he did extrude midplane. TIP: Since you are new to Solidworks, make it a habit to extrude bosses MIDPLANE, and you will save very much time and effort especially when you inevitably need to mirror features.
2. While still on the front plane create another sketch that will start from the bottom on the cylinder and sketch a straight up to the bottom of the boss then sketch an arc at the top of the line following the bend of the example picture. TIP: You can save time sketching arcs at the end of straight lines by clicking a stopping point then moving the mouse up and back down to the line and you should automatically be in arc mode or click the end of the straight line and press the a key. This line with the arc at the top will be a path. click the sketch in the directory tree and press F2 to rename and name it PATH.
3. Create a new plane using the top plane and the bottom point of the path sketch. or you can select reference geometry>plane and select the sketch line then the bottom point to create a plane for the bottom of the cylinder.
4. Draw a circle for the cylinder on the new plane slightly off center dimension it the move you view angle so you can see the path line. Now select the center of the circle and CTRL select some part of the line then in the small dialog box select pierce for the relationship and the unattached circle will snap to the end of the line. TIP: It is best to use the pierce relation for profile sweeps. Again when you close the sketch click the sketch name in the tree and F2 then rename to PROFILE.
5. Now activate the SWEEP BOSS command and select first Profile then for the second field Path. The sweep should look like your example picture.
6. All that is left is to cut off the square end of the first boss to match the cylinder. Here is a trick for that. Click the bottom of the cylinder and normal to however you have it set up. TIP: if you wish to control normal to at your command, but save time go into the set-up options and set the spacebar hotkey setting from bringing up the view dialog to directly use the normal to command. This has saved me so much time and effort. By unchecking the option for automatically making a sketch normal to on creation or edit, I can just hit spacebar when I want it or sketch in my current view which I often do with sweeps. Now to make the upper boss cut select sketch on the bottom of the cylinder and select the sketch circle for the sweep and convert entities. It will copy the circle to this sketch. Slice the circle in half with a centerline and use the trim tool to trim away the inside of the circle. You can exit the sketch and select cut extrude and you should get a surface cut that will give you the final shape.
7. making the thread uses another sweep One you create the thread boss, chamfer the end of the boss at 30°, create a path sketch of a straight line down the boss on the front plane. name it Path2. for now just make another sketch of a v shape at the end of the thread boss. If you feel ready to model with equations I will send you a sketch which makes any size thread profile using the UTFS/ISO standards. It uses equations to make the calculated profile for each thread size. So for noe sketch the v shae on the front plane and make the top of the v co linear to the top of the thread boss and match the inside of the v to the chamfer. make the angle between the two sides 60°
and make the sides equal relation. close sketch and name it Profile2 or "thread profile"
8. Activate the sweep boss tool and select profile2 then path2 then in the options section select twist along path from the drop down and then select turns. Now work out what thread size you have and how many turns it has per inch for example a 3/8-16 bolt has 16 turns for each inch. enter the number of turns and you are finished.
Well, I just wanted to show the result i got thanks to your help!
Answered with a tutorial: https://grabcad.com/tutorials/approach-to-model-this-tap-in-solidworks-2012--2
Wow guys! so many responses Thank you all!! Where's the give a beer button? Actually, I followed everyone's approach to gain practice, thank you Kent, thank you özgür and thank you Rollin (what a piece of text!)
I managed to actually get what I wanted to get. Now, a section view problem arises. Should I open a new thread or is it ok to post it here?
Very nice. Is the knob on the top a pump actuator or a twist valve?
Thank you Kent, yes it could be a pump actuator, it's the knob of a temporized faucet, I attach pic :-)
Answered with a tutorial: https://grabcad.com/tutorials/approach-to-model-this-tap-in-solidworks-2012--3