pattern of part along a curve

[Indusign]

For this new project,I need to pattern the links of a track along the curve they will follow. I can get them to pattern along a curve, first made the curve, then placed point on the curve with 'on curve, lenght ratio', patterned the point, then assembled the track link. But it allways keeps the same orientation, how do I force it to follow the curve ?

 

[skraba]

My guess is, create another pattern of points offseted by link length and assemble the link to two points.

 

[Indusign]

Hi skraba,


Hmm as you will know by now nothing in ProE is that simple. This is the result I got with the methode you described. Second point was also on curve and ofsetted.

thanks anyway for the advise.

 

[sivaraman_45]

hi,


can you try in this way.


As you created, Place a point on curve and pattern it. also create an axis on a point and tangent to the curve.


Use this Axis for the Alignment of your link and ref-pattern it.


The Link may will turn acco. to the Axis' direction.


Pls reply whether it works fine.


View attachment 1138


regards,siva
Edited by: sivaraman_45

 

[ProE_Addict]

I just hada similar issue, though not in an assembly. Mine was patterning a feature on a curve and I wanted the feature to remain tangent.


Here's how I did it...


Create the curve you want your pattern to follow.


Create a copy of the curve just created and select the "approximate" option, rather than the default, "exact". The use of an approximate curve essencially creates a spline curve over the original.


Create a point on the approximate curve.


Create a sketched curve. In this feature, first sketch a construction line through the point and tangent to the approximate curve. Then sketch a solid line through the point and normal to the construction line.


I then created a datum plane through the normal curve to use for positioning my sketch.


Create your feature to be patternedand Shazam!

 

[slashct]

I think I know what you are trying to accomplish and there are some limitations, I'll try and explain. I did for someone a cable track where cables go inside the track and the links move along a theoritical curve. The problem that you have is that the links are straight and if you go along a curve you cut the curve off short. Also one thing that happens is that the links will hit a dead spot so to speak when they fall in a certain position, in my case it turned out to be4 links would really shorten the curve so we had to watch the increment and put a relation in to stop this.
In the end when you create the curve you need to make sure that you drive the length of the curve by using the perimeter option, and now you take your link length and a multiple of the links, do this with a relation. Doing this makes sure that the length of the curve will be the proper length (if everything falls correctly). You can than use the ratio option on the curve to create points because you are driving the length of the curve and than pattern the points.Without seeing what your trying to do not sure how you would want to assemble... You can than use joints to assemble the links, problem is now you need to do this for each link..
This is what my assembly ended up looking like:


View attachment 1141

 

[paltsten]

At www.ptc.com there is a suggested technic for this one:


"Suggested Technique for Modeling a Chain Assembly"


Or you may install Wildfire3.0 and thy it out, its soooo easily done... in the future

...member orientation...follow curve, se picture


//Peter


View attachment 1151

 

[Indusign]

Hi palsten,


I can't seem to find that technique on the PTC site, can you post it here ?


We use 2000i2 here, so the Wildfire solution isn't an option.

 

[Indusign]

Hello all,





Just placed them all by hand, only on the straight lines I used a pattern.


This is the result: