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endlasuresh

cone shape with lines

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endlasuresh

Hi,

I am back after long time because of some loss in company, anyway i am looking to start again and forgot all those things that I learned from here. Still I remember got excellent help from the person here (name forgotten).

 

 

Anyway I will be here for a long time because looking to buy injection mould.

 

 

Presently I am looking to draw a water spike, but the lines aren't getting in my mind how to do. I drawn cone shape, in less than 3 mins.

 

 

 

attachment.php?attachmentid=57173&cid=1&stc=1

Edited by endlasuresh

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shift1313

Welcome back suresh! It might be because I am viewing on my phone but I am having trouble viewing what lines you mean. Is the cone straight or defined by an equation? What shape is the lines profile?

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endlasuresh

Hi, thanks for the reply, Yeah I got all the help from you.

 

I mean the lines are on the cone, you see one on the above image and the rest are covered in back. The four lines are drawn using linear mode in equal length on the circle.

attachment.php?attachmentid=57178&cid=1&stc=1

 

Ill get my diagram in the next post as SolidWorks is on another system.

 

here is my drawing

attachment.php?attachmentid=57182&cid=1&stc=1

sddsss.jpg

Edited by endlasuresh

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endlasuresh

If you are unable to view the above image then please look at this because it is not showing on my laptop.

attachment.php?attachmentid=57183&cid=1&stc=1

 

The line thickness is 1.2mm and depth is 1 mm and the line slowly decreases while moving towards to the top end also the depth too decreases.

I think in the middle is somewhere .6 mm

There are 4 lines in equal length around the cone. I think we can use circular pattern but on a cone I am not getting.

scopy.jpg

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shift1313

Suresh, one way to do this is by using Sweep. You could also do it with just an extrude cut picking a reference direction. I will detail the sweep method with text and a few images because i don't have the time to make a video right now. If you have any questions let me know.

 

After your cone is drawn you want to make a sketch on a plane that bisects the cone. If you drew the original revolve on the Front plane just use the Front plane to keep it simple. In this sketch you can either grab the original revolve sketch or use the "convert entities" drop down and select "Intersection curve. From here you will have the outside edge of your cone.

 

The next step is to draw the "path" you want to cut the new feature away. You want to make sure any geometry you got form intersection curve or from the original sketch is converted to construction geometry. You want to draw the path with a line that starts inside of the cone(i used 1.25mm since this was the number you gave) and then dimension this line to exit the cone shape where you need. I also added a 5mm long straight line past the base of the cone to ensure i get a nice cut. exit the sketch

 

Next you want to create a plane by select the end point of the 5mm long line and the line itself. This will make a plane that is normal to the line.

 

Now start a new sketch on this plane. You want to draw the profile of what the cut needs to be. If using a circle i like to add a reference line from its origin to the quadrant point we are going to use. This lets me also have a horizontal(or vertical) relation on this reference line. If the shape isn't a circle this will help make sure its fully defined\located. You want to take the end point/quadrant point and the 5mm line and make a "pierce" relation. That should fully define the sketch. exit the sketch.

 

Now because the profile was drawn on the "normal" plane to our path, and the path is a straight line you can just Extrude cut it "through all" . You could also do a sweep cut. you will have to play with the dimensions of your reference sketch and the size of your cut profile to match what you have but that is the process.

 

Note, if you use an extruded profile from a plane that is not normal to the path you can pick a direction by selecting a line in the box just below (blind). This will give you slightly different results since your profile will not be a true profile since it will be extruded at a slight angle. I suggest making the reference sketches mentioned above to accurately control the path and profile.

 

I added a few images below for you. There are many different ways you can achieve this though. You can use a loft going from your profile to a sketch point as another option. The end result will be the same it just changes based on what your inputs are and how you want to control/update it. I can make a video for this process tonight showing a few methods but let me know some more dimensions. I need one more dimension to fully define the cone(height of the overall cone) and if you know the height where the cut feature exits the cone i can make some accurate reference sketches. Is the cut a circle? 1.2mm diameter but only 1mm deep into the cone, or does it appear to be something more complex?

Sketch1.jpg

Plane1.jpg

Circle.jpg

Cut.jpg

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endlasuresh

hi thanks a lot,

cone height is 122.5mm

top of the cone dia is 3mm

bottom of the cone is dia 22 mm

The lines thickness is 1.2 mm and depth is 1mm.

This will undergo in the CNC wirecut as they have asked me to get the diagram. The lines are just for looking beautiful, also to make hole easily.

attachment.php?attachmentid=57190&cid=1&stc=1

 

I made a closure picture and you will see the lines are very light at the top end of spike. i will give a try by using your above method.

spike.jpg

Edited by endlasuresh
double images

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shift1313

give it a shot and let me know if you have trouble, then i can make some more references/video for you. FYI the double image, when you upload an image it automatically attaches it to the post. If you select "insert inline" then it also puts it in the body of the post. Thats why you have a double image.

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endlasuresh

i tried both the ways by using loft method too and it is more easier using loft method. As per your tutorial i went through the intersection curve but didn't made any geometrical. I understood what you meant is draw One circle at the bottom of the cone and the other top of of the cone and it should proceed in the path that is the line.

 

ill give a try again and see.

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endlasuresh

I tried all the day by front plane method, but this is not making the sketch where it required. I tried to draw a circle at the end and top of cones using front planes, but the were getting in perpendicular direction instead of opposite.

I think I am missing something at here.

 

The line was just like a thick line with 1.2mm not 2.5dia.

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shift1313

So you made a "path" that was 1.2mm inside the cone, a plane off the bottom of that line, amd a circle on that plane which its upper quadrant intersects the line with "pierce" but its not working? I can make a quick video tonight.

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endlasuresh

I drew a line as you did it, but here the line starting point doesn't make a circle. I kept the line far to the cone bottom, but the plane is touching to the cone base any thing goes at this point instead of on the starting point of line.

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shift1313

Suresh, remind me what version of solidworks you are using.

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endlasuresh

Its Solidworkd premium 2010 i will give a try again. I think i missed the path as it says Nothing is selected that is suitable for the path.

 

I some how managed to draw a line and sweep on it will post again within 2 hours.

Edited by endlasuresh

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endlasuresh

In the end I made a cut on this cone without measurements roughly done, but here the other end too went in same depth.

By linear circle also this swept cut doesn't cuts, I might missing more things.

I made through reference geomentry and then Swept cut.

Can you let me know how to make adjustments of the other end as it should be 0.2 or 0.3 line and remain on the top of cone.

image.jpg

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shift1313

I was hoping I could send you a file but I haven't had 2010 installed on this machine ever. I'll make you a video tonight. I was too busy last night. I think your path sketch is the problem.

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endlasuresh

The path was the main problem,never drawn such type, but 5 years while I was on this forum did a Gear with the help of you.

i saw the video and it has more helpful for making extrude cut using a path. You have did as per the image, but had to change as per the cone.

Iive did a triangle and want to place it on the cone for extrude cut as this is the correct thing. The top end touches to the top of cone 3 mm dia circle and bottom of the triangle base 1.2 width touches to the cone of dia 22

 

The bottom of the triangle goes into the depth of 1 mm extrude cut while the other end stays on the top of cone.

Th slopes are made automatically and we don't need to add a line or anything.

let me know how to place this triangle on the cone?

 

image.jpg

Again here the measurements and a clear shot for you.

Cnc Wire thickness is 0.2 so the top end of triangle will be 0.2 and bottom of the triangle will be 1.2 mm width.

At top end their is no depth

at bottom of cone is 1mm deep.

image.jpg

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shift1313

suresh, in the video i sent you the end result cut was tapered. I had the dimensions wrong but if you make the rectangle at the bottom 1.2mm wide and 1mm deep (adjusting the sketch path to be in 1mm instead of the 1.2mm i did) into the part then the one at top 0.2 wide and loft cut between them you will get your shape. You can also draw your cone sketch and do a projected curve or split line on the cone to use as guide rails in a boundary cut or sweep cut.

 

so the difference in the video i sent you need to take the sketch path up to the 3mm section up top and not 5mm down like i did. The process will work other than that dimension and whatever changes you want to make to the rectangles. Am i missing something here?

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endlasuresh

I think all is well, but morning will give a try and the final question do i use circular mode for making 4 lines on this cone? I tried in the last diagram and it placed all in serial row touching to each other.

 

This time ill try as you mentioned in the above post will let you in early morning.:D

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endlasuresh

I got it in the early morning within 10 minutes using loft cut method, but was away before posting here. Here is a screenshot of it, but Ill post the plates once it processed, I think on monday or tuesday their would be some pieces in my hands.

cone2.jpg

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shift1313

great job!

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