How to model tri-angle teeth around a tube end

[oldboot]

I tried to search similar topic but failed. I a new guy and have a stupid question.

I have a component which is a regular tube, but one end of the tube is tooth-shape, the 16 saw-shape teeth connected one by one around the circle. I could not use any straight cut as the tri-angle shape in outer surface of the tube wall is larger than inner shape.

Is there anyway to make this happen? ---I thought several nights---this question sends me to dream every night---but still do not know how to do it.

Hope I made myself clear enough with my English as second language.

 

[ctopher]

Try extruding one tooth from the end then array the feature around the diameter.

 

[APPENG]

Graysony,

I have done this very same thing with the same conditions. What I wound up doing is creating a "v" shaped surface using a loft. There was setup work here using construction sketches to help me define the loft sections. Then after I created the loft, I used the Cut with surface command and then created a circular pattern of the cutout using the temporary axis of the cylinder as my axis of rotation.

Now I used surfaces on this example but you could also use a cut loft as well.

As far as the pattern goes, you find that you need to check the "Geometry pattern" option.. but only if its necessary, and it will tell you when it is.

hope that helps


Regards,
Jon
jgbena@yahoo.com

 

[oldboot]

Thanks for your help, but to my understanding to your words, it is not what I need.

If I extrude one tooth, then the tooth will grow 'straight' up from the end and bulid up a straight surface on body side, but the tube wall is curve surface. A straight tooth wall and a round/curve tube wall does no match----I need the tooth wall to be the same curve as that of the tube.

Is there any other way...if I understood your words correctly?

 

[APPENG]

No actually that what the construction sketchs are for... so that you define the angle of the cuts such that they are perpendicular to their intersection on the round face.

When you make the cut, its actually tapered if you take my meaning..



Regards,
Jon
jgbena@yahoo.com

 

[TheTick]

Make a cylindrical surface that matches to tube I.D. or O.D. Cut the tooth shape into the cylindrical surface, then use thicken to create the solid.

Maybe you could turn the tube into a sheet metal part, unroll the tube, cut the teeth, then roll it back up? This will require that a seam be put into the tube.

Due to illness, the part of The Tick will be played by... The Tick.

http://www.EsoxRepublic.com

 

[oldboot]

Thanks APPENG, my first reply is for CTOPHER. He is also right with your detail information. Now I understand there is another 'cut' step against the lofted/protruded tooth.

I will try the way TheTick says as I have another problem if I do your way: the LOFT.

I found any ends/section of a LOFT must be a 'closed' shape/sketch such as a circle or at least a triangle.... But for a 'V' shape loft, we need a "sharpe" end. It is a line--like the keen of a knife, or only a point---like the top of a paramid....So, how to creat a loft with sharpe end?

Do I must use mold tool? Put something with sharpe internal angle to a cube/body and substract/dig out the cavity to build that kind of sharpe top?

 

[MElam]

If I understand you correctly, you could do this using Sheetmetal tools as Tick mentioned. I've done this before for non-sheetmetal parts:

1. Draw the tube profile as an ALMOST complete circle (leave a small gap for a seam - to be filled in later)
2. Use the Base-Flange feature to extrude the tube. Under Sheet Metal Parameters set the tube wall thickness and use the "Reverse direction" box to control wheather the sketch should be ID or OD.
3. Use Unfold feature to flatten the tube (select EDGE of seam when asked for Fixed face)
4. Create teeth in the flat.
5. Use Fold feature to roll tube back up.
6. Fill in seam with extrude feature.