I have been asked to model this corkscrew in solidworks. Will need to be assembled eventually. Would be grateful for some help on this basic steps for each component would be a awesome. Thank you.
Here is the hanger bracket
There are measurements missing from your drawing so i had to guess some of the dimensions. This should get you started. The nut is the most challenging part as there is a twist in the handles.
Here is the swivel
Great start & Help Paul. thanks so much.
Here is one way to model the screw
Great stuff Paul. Thank you kindly. I modeled the hanger bracket, apologise about the missing dimensions. I believe these to be correct, Hopefully the model is accurate. cheers
your hanger bracket looks good to me, one thing I noticed is that your boss extrude 1 is only 50 mm long the drawing shows 75 mm long, your modelling technique is good.
Many Thanks I changed the dimension to 75 and now have issues with the swept size. I sketched a new swept path and using the guide curve as the new sketch and getting error or it only sweeps half way down. any ideas? please find attached.
Also having an issue with this drawing, could you briefly walk me through it, Im unsure how you're getting the 17.25 dimension, from what line is it taken from considering the back is round?
I have created my sketch on the top plane.
Then when you look directly down on the top of the part SW will allow you to dimension from the virtual edge of the curved face, By using coincident and tangent relations the only dimension that I need to fully define my sketch is the 17.25 mm dimension
I am having a look at your hanger bracket
The first thing that I have to say is always make sure your sketches are fully defined If I look at your sketch 4 you will see that all the lines are blue and that the lines I have circled in red are not in the correct position. they should be colinear with the virtual edge of the cyliner
Always make sure and add either sketch relations or dimensions so as to fully define your sketches.
Your sweep will not work when using a guide curve because the difference between the 2 dimensions is too great and the outside fillet is now further away from being concentric with the inner fillet and the profile of the sweep cannot be maintained when creating the sweep
As you already have your sketches drawn the easiest way to create the part is to do a sweep and a boss extrude
First edit your sketch 4 and add in 1 new line
Then edit sketch 5 and add 2 new lines
Now create your a sweep, when you go to select your profile right click in the top box highlighted below and choose selection manager this then allows you to select the sketch lines from sketch 4 that you want to sweep
Select the lines your want to use as the profile and then select the green check icon on the selection manage tool shown in the graphics area. You will also be able to use the selection manager to select the path to sweep along from sketch 5
this will now give you this
Now using sketch 5 do a boss extrude
Many thanks Paul that's excellent help I am most grateful. Unable to do the last midplane boss extrude on that hanger bracket (attached)
Attempting to model the screw now, perhaps you can see if I am on the right path. thanks kindly. (attached)
If you zoom in on the corner highlighted in red you will see a small gap between the lines
If you look normal to your sketch you will see that the line with the 82.88 dimension is not vertical, delete the 82.88 dimension and give the line a vertical relation and the gap will close and the boss extrude will work
On the screw your sketch 21 is not fully defined make sure and fully define the sketch
I can easily pick a point and drag the sketch out of shape,
make the construction line horizontal, give the end points of the construction lines mid point relations to the 2 vertical lines. make the line on the left hand side vertical as it should be the line on the left should be dimensioned 1.2 mm make the bottom left hand corner of your sketch coincident with the bottom corner of the extrude. When sketching in SoldiWorks you need to use relations as much as possible and dimensions as little as possible and you always need to fully define your sketches
In your sketch 22 the end point of your line is not fully defined, you have to fully define this or when you go to make the thread if the end point moves it will mess up your thread.The point is blue this means that it is not fully defined you can fully define it by making the point coincident with the end of the boss extrude or be giving it a dimension. The reason why you should do one or the other is as follows, the length of your threaded area will always be whatever the length of the line is. If you make the point coincident with the end of the boss extrude as you make the boss extrude longer or shorter the length of the threaded section will also update. If you give the line a dimension the length of the threaded section will always stay the same even if you make the part 2 times as long as it is now. You need to decide which is the best way to go. I would go with the dimension as you will not want the thread to distort.
Many thanks Paul this is an amazing resource and help for everyone.
I believe the bracket is now modeled correctly (attached)
nearly finished the screw, the second cut sweep dosent want to work for me (attached)
And the swivel is almost finished just very unsure what I am supposed to do after doing the plane (attached) The drawings are unclear for a novice like myself.
Cheers Paul !!!
In the screw you have a vertical line in sketch 21 that you do not need, delete this
The line that you have drawn in sketch 24 is a construction line you need to change it to a solid line and then the sweep will work by selecting sketch 21 as the profile and sketch 24 as the path.
In the swivel the reason I created the plane is to sketch a slot on it so as I could cut away the part as it required. How I created the plane was to select the line and end point of my original sketch 1 and then go "Insert - Reference Geometry - Plane" a plane is then created at the end of the line and normal to the line, note: the plane is created at whichever end point you selected.
Now I created a sketch on the plane
Now I cut away the material that I wanted to remove by doing a cut extrude with an end condition of up to surface and I selected the face of the hole passing through the part
This then gives you the finished part
In the hanger bracket your sketch 5 has a line and an arc that are not fully defined,
You should always check that your sketches are fully defined (blue lines or points ect. = not defined, black lines or points etc = defined) this should be one of the first thing your teacher tells you before you even started sketching in SW. Have a look at this video
or here https://www.youtube.com/watch?v=-RORuZoj2ag
As you can see I can easily pull that sketch out of shape and then your part will be wrong. Give the line a vertical relation and make the arc tangent to the line.
When I look at your sketch 4 it looks incorrect to me. it is off center and the 6 deg taper on the bottom section is all over the place
Have a look at the attached video for what I did to repair sketch 4 and 5
I am sorry if you think that I am being a bit vague. I just wanted to point you in the right direction without telling you too much, sometimes you learn more from the blood sweat and tears that come with figuring something out for yourself than from somebody showing you how to do it.
Great help Paul The video is very good thanks
Getting rebuild errors when I sweep cut the screw (attached)
Not sure how you were able to select the top line in your swivel sketch sketch 1 as the plane option is greyed out in edit mode?, also unsure how to get the dimension of 1 at the top down to make it defined (attached)
On a plus note I believe the hanger bracket is finally correct thanks to you, yayy!!! (attached)
Hi Paul. Have attempted the Corkscrew Nut, If you had some time that view it that would be great.
It looks good so far, now you need to add the 2 "wings" to the nut
The first thing I did was to sketch the wing profile on the end of the body
I then created a reference sketch on the front plane. This sketch will be used to set up a plane at the angle of the end of the wing
I now created a plane for the sketch the end profile of the wing onto to
I now created the sketch of the end profile of the wing on my new plane
I now created a loft between my 2 profile sketches. Merge the loft with the body
Then mirror the loft feature to the other end and add fillets as required to finish the part
Amazing Paul thank you couldn't have done it without you!! Seems to be correct (attached)
Now onto the main body (the last part) not sure where to start with this perhaps you could give some pointers would be most grateful.
The nut looks good
The body is just a revolve followed by a cut extrude
Amazing Paul thank you. I'm having offal trouble adding double distance dimensions to the rest of the sketch can you have a look and see what you think if theirs anything obvious.It keeps over defining the sketch. many thanks
You have relations in your sketch that is messing things up for you. You will see in the picture below that the line for the inner diameter has a collinear relationship with the line above it. you also have 2 coincident relationships with the end points of the line above it. Delete these relations
The top end point of the same line also has a coincident relationship with the line above it. delete this relationship
The same goes for the bottom end point of the line
You also have a tangent relationship that needs to be deleted
Thanks Paul. I just deleted all relations and got most of the dimensions done and only added some verticals to stop it going out of line. lesson learned here for sure. I believe it to be correct, it looks good and can be worked on, this has been a great help Paul a big thank you for all your help in getting this done, hats off to you sir. cheers
I have to assemble the parts together now and get some motion with each other, should be fun
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