concentric pattern

[KenMagnnetic]

I am using solidworks2004 can anyone help me i need to produce a series of concentric grooves in a Part each 3mm apart ( each groove 6mm larger in dia than the previous) from 50mm dia upt to 450 dia. Is there a pattern or quick way because otherwise i have to cut extrude each groove seperatly(66 times) which takes ages

 

Thanks

[CALCAD]

Kenmagnnetic,

I am using Solidworks 2008, so I don't know if you have this capability, but the displayed image was generated from a simple sketch of the groove profile that was processed with REVOLVED BOSS/BASE in one operation. Can this be done with Solidworks 2004?

[CALCAD]

Or maybe like this with a set of grooves applied to a surface with the REVOLVED CUT command. This image shows the sketch that was revolved.

[KenMagnnetic]

Hi Calcad

 

Yes that is what i am trying to acheive did you do a linear copy of the revolved sketch or did you create anoter plane on the centre line on which you made sketch of the groove. I seem to only be able to do linear copy of features not sketches.

 

Thanks for trying to help i only know the basics

 

Ken

[CALCAD]

KenMagnnetic,

I'm not an expert with Solidworks. So it took a few tries, but I was eventually able to draw a sketch

that used LINEAR PATTERN to produce the row of teeth that was used by REVOLVED CUT to produce the image shown.

If you don't have the LINEAR PATTERN option for sketches in Solidworks 2004, an alternative might be to draw the entire

row of teeth manually. But it's not as much work as it sounds, because you don't need the teeth drawn

precisely. They may need to be drawn square, but the dimensions aren't critical because you can (I think)

use the EQUAL option of ADD RELATIONS to make the dimensions uniform. I was able to do this as long as I drew

the first tooth with precise dimensions. Then after a few trial and error cycles I could force all the teeth

into a uniform pattern. I am assuming that you do have the REVOLVED CUT feature option. I hope this helps.

[shift1313]

the way calcad drew this is a good way to do it(in my opinion). I am not sure if there are any options available to pattern something as well as scale it at the same time. revolve cut would be a good way to know your getting the correct feature.

[KenMagnnetic]

Calcad /Shift

 

Thanks for your help. I can produce a single revolved cut with no problem, but i cant linear pattern this because it make no allowance for the reduction in diameter for each concentric groove. I just end up with the same groove moved sideways. I do not have the option to linear pattern the sketch only unfortunately. Looks like ill have to put each groove in on the sketch like clacad said with the add relations equal option, still going to be long way tho because my model needs 38 grooves.

 

Is it possible to linear pattern sketches in newer versions of Solid? Not sure if i can afford them tho

 

Ken

[shift1313]

ken, as your grooves go out are you trying to change their elevation as well? or are the widths of the groove just changing?

[KenMagnnetic]

No the grooves i want remain the same dimension ie 1.5mm wide x 1.5mm deep. My smallest diameter groove will be 50mm OD the next groove will be 59mm OD then 68mm OD ,77mm OD....etc

 

K

[shift1313]

i have never used solidworks 05 but i just drew this up quick in 08. I first drew a circle, extruded it. then i sketched a rectangle and a line(to revolve around). I dimmensioned the rectangle so it was 1.5mm wide and 1.5mm into the cylinder. Finished sketch and used revcut to make a groove. Then i went back and edited my sketch(could have done it at the initial sketching) and used linear pattern. I entered my offset values(4.5mm) and 15 for number of copies.

 

If you dont have linnear pattern in your sketch tab you will have to draw a single sketch with the 2d profile of all your cuts. with the equal constraint under add relation this shouldnt be hard. You also should have copy entities available to use.

[KenMagnnetic]

Yay!! i did it thanks for your help guys

[shift1313]

your making a rotary table:)

 

glad you got it worked out. did you have an option for pattern?

[KenMagnnetic]

Its actually the top plate for an electromagnetic chuck.

 

i used the copy entity feature in sketch then revolved cut. I hadnt used the copy entity b4. You know what its like when you learn the basics yourserlf never seem to try new things just stik to what you know. But i learnt somthing new now.

 

thanks again.