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Pattern in assembly using a sketch

Hello I am trying to create a pattern of parts in an assembly but the pattern is irregular, just positions with no feature to back it up.

 

I've attached an image.

 

I need to pattern the bronze bolt accordint to the sketch, but I can not create any features on the plate.

10 REPLIES

Re: Pattern in assembly using a sketch

[ Edited ]

@JasonTitcomb had posted a Pattern Template few days back. Read it here.

I wrote an article about it on my blog.

 

Hope you find this relevant and useful.

 

~Tushar Suradkar

www.CADVertex.com

Re: Pattern in assembly using a sketch

Hi,


as I interpree Your picture, it seems for me, that You want to pattern bolts.

So if there is a hole pattern in the part, then You can use it for patterning the bolt in the asm.

 

regards

Wolfgang

 



regards
Wolfgang

Re: Pattern in assembly using a sketch

thats not really the case ... those bolts will be welded by a CNC welder and there is nothing except some coordinates that marks their position on that plate ... so the only thing I can do is a sketch where I mark with points (or circles) the position of those bolts

Re: Pattern in assembly using a sketch

Hi Norbert,


so, try it as following:

 

Even if there are no holes in Your part, creat a hole feature.

But now, detach them.

So You will get a surface hole feature, which doesn't change Your part, but is a valid feature for patterning within the asm

 

Works fine for me here!

 

regards

Wolfgang

 



regards
Wolfgang

Re: Pattern in assembly using a sketch

[ Edited ]

Hi Norbert,


forgot to mention:

this will work in synchronous that way!

 

Haven't found a way to do similar in traditional

 

regards

Wolfgang

 



regards
Wolfgang

Re: Pattern in assembly using a sketch

Hi,

 

 

 

there will be a method for a pattern without a corresponding hole feature.

 

Create a patternb along a curve witihn Your ASM.

 

Here You - for a very long time - have the possibility to insert additional accurences on vertex point of Your cure.

 

If Your "curve" will be a set of straight lines, this is a very simple task then.

 

regards

Wolfgang

 



regards
Wolfgang

Re: Pattern in assembly using a sketch

I have to dimension the points in coordinates from the lowest point to and the right side of the plate.

I did try the curve pattern but I only saw the option of fixed dimension between points

Re: Pattern in assembly using a sketch

[ Edited ]

Hi Norbert,

no, start with chain selection of Your line set, giving 2 elements for fit.

This brings You one instance at the beginning and one at the end.

 

And then look for the last icon "Add occurence"

 

 

Then You can select every vertex point on Your lines to add additional pattern instances,
which give You for instance a result as following

 

 

 

regards

Wolfgang

 



regards
Wolfgang
Solution
Solution
Accepted by topic author NorbertS
‎10-08-2015 01:52 AM

Re: Pattern in assembly using a sketch

Hi,

 

I've solved this challenge on part level. What does this mean?

 

You can use Pattern by Table in synch and ordered too. Other solution is what was mention by @hawcad detaching holes, but this works only synch mode.

You have mentioned that you need a solution in ordered mode. Yes, you can do this in it, the key thing is the "multibody" modeling there.

 

 

Here is a video and it contains all solutions what was mention by me:

1. Pattern by table (both) 0:00 - 5:44

2. Detach holes (synch) 5:45 - 11:38

3. Multibody modeling by holes (ordered) 11:39 - 16:06

 

I hope this help!

 

BR,

 

Imics
http://solidedgest.wordpress.com/