[Craigpat]

I am designing some solid wheels for an rc car every thing is prototype at this point. what a am tring to do is wrap a tread pattern around a wheel and have them evenly paced the spaced. it looks fine except for where the first and last tread meet. i have done this simply by making a linear pattern and doing the wrap feature. this is done fairly easily. im not sure if i should use an equation (radis or divid # of treads into 360 and adjust the angle between each tread)to adjust and get proper spacing prior to wrapping. Or is there a more intuitive way for this to be done before the wrap is used? note: im usin a V shaped tread or some other type so i dont think a circuler pattern will sufice. I am a self taught SW user so if there is a feature that i am not aware of let me know

see attached pics to get a better idea of what im doing

thanks for the in put
Craig

[pixburghenat]

Hello,

On your model I'm assuming you want 24 cleats, 360/24 = 15 degrees

When using a wrap feature the linear pattern has to be sketched with the circumference in mind. Such as if the diameter to be filled is 4 inches, the linear sketch length to fill, for the wrap, would be PI*4 = 12.566370614359172953850573533118
So your distance between would be (PI*4)/24 = 0.52359877559829887307710723054658

(The numbers were cut and pasted from the Windows calculator)

I always use the equation in the dimension input box, any rounding will accumlate an error.
Check your sketch fill length or distance between, it may be a little short and it could be why your angle didn't equal 15 degrees.

You could also try sketching and extruding upto the disk surface one cleat and then use a circular FEATURE pattern. Using the feature pattern, you only need to select the feature you want to pattern, the center of the fill pattern, how many copies, and then 360 degrees to fill. You could also use the offset from surface and it will create the cleat with a round top that follows the tire diameter.

Scott

[pixburghenat]

A quickie.


Scott

[JerryFlyGuy]

Wouldn't it be easier to model the first thread on the top and then do a circular pattern of the thread around the wheel. It'd be parametric so if you ever change the tire size for some reason, it'd update and still be patterned around the tire at the same angular positions???

Curious..

Jerry

[cadman]

X3 on the Circular Pattern.

[Craigpat]

ahhh i do lovve a good debate
idid think og feature patern on the way to work today. Waht i like about solid works is you can do things in more then one way. some can be easier then others. great ideas and i will try them out

cdman,
x3 on a cirular pattern ... i dont understand?

than you for your time
Craig

[cadman]

I "third" that (third person to agree).

[Craigpat]

Great istructions guys i am getting good results from it. had to ply with setings due to disjointed error (but i over came this silly error and pressed on) i have made a stipled wheel as well. going to be interesting to see how the car handles with solid heavy wheels

see pic, not good for carpet awsome for dirt


a question for the mod,
why doesnt the forum allow fow straight upload of sw files? they are rather small and would save astepp renaming ect ect. just curious thanks
craig

[JerryFlyGuy]

ahhh i do lovve a good debate
idid think og feature patern on the way to work today. Waht i like about solid works is you can do things in more then one way. some can be easier then others. great ideas and i will try them out

cdman,
x3 on a cirular pattern ... i dont understand?

than you for your time
Craig

Ya this is true, generally there is a easier/better way and a harder/less efficient way. I repeatedly remind SW users to not think in an 'AutoCAD' mindset. The wrap idea is just that, a route that would be taken in if a person was drawing it in AutoCAD, in the world of SW, try and use it's feature base and parametric's to your advantage.
ie; doing a wrap, each time you change the DIA of the wheel or the # of tread instance's you have to redraw the wrap. If on the other hand, you draw one tread and then pattern it around the wheel, if the wheel size changes it will update automaticly [granted you modeled it in a way which allows it to do so] if you want to change the # of instances on the tread.. again two mouse clicks and it's done.. no math.. PERIOD.. the guy's who work w/ me [newer user's] are amazed at the time savings when the easier route is followed.

Most of us are old AutoCAD user's so it's an easy rut to fall into, I've had to fight my design tendancy's since I started using SW, it's soo different and better, we just have to adjust and exploit it's power to our advantage.

Feature base parametric software has changed the whole CAD game [from 2D CAD], if it's used to it's full advantage it's more efficient and fluid, if it's not.. it's generally no faster than AutoCAD as a person has to 'redraw' all the time..

FWIW

Jerry

[pixburghenat]

Hi Jerry,

You are right, parametic is the way to go.

I did have a project last summer that used 2 helixes to create 1 sweep cut.
I messed around with that for a couple of days. I could create the sweep path without a problem, but when the cut sketch was applied, the results were not what I wanted. The cut path twisted along the sweep and closed the groove a little. I tried the keep normal to and all of the options of the feature, but no go. I ended up doing it the old way using a wrap feature, worked perfectly. That was in Solidworks 2007.

Today I've really started using 2008 and I tried the same helix sweep cut again, now it worked the way I expected.

Scott

[Craigpat]

i started using a regualr 2d cad called cad standard trial version free and was a good start ...$20 bucks for the whole thing.. You could even projet isometric veiws to get a good plan for my wood working. I tried autocad and then turbo cad. i just couldnt figure it out. Then i saw solid works (ahhh beam of sun light coming through breaking clouds , god showing you the correct path :wee: ) i went throught the tutorials found some dvd courses Tadda . now i do full 3d models for projects.
I to have been playing around with helixes very cool. they will make awsome cnc cut legs of things. For a new user i consider mysef pretty accomplished. took a month or so to get a real handle of it,

attachend are a few things made.. primaraly i made everything as a single part which works for me

thanks , enloy
craig