I have a cylindrical part of which I require 70 at even spacings around an arc. Pattern you say? Unfortunately each one is required to be increimentally shorter than the last by approximately 17mm. Shy of making them all individually can anyone recommend a better way?
Picture below: The tallest pole at the left is required to be 1300mm tall, shortest on the right required to be 100mm tall, but all must be flat on top (otherwise a swept surface and subtract would have been ideal). These are tubes with a welded cap on the top for context.
Thanks in advance for your thoughts & suggestions.
Solved! Go to Solution.
If you use frame members and extrusions (ordered, assembly), could save you some time. Then you only have to change the line/sketch length for each one that could be done quickly with some relations and variables shortening each line as it goes around the circle.
Then extrude them all using the same profile, but varying extrusion lines.
try the steps shown in attached video. I did it on extruded part, but as 12GAGE suggested, you can use frame component as source for pattern. Then create a pattern curve in new "dummy" part. Finnaly pattern frame member using curve and cut all members except first one with Assembly Feature Cut.
Only problem with this method I can not achieve that one pipe is approximately 17mm shorter then next one.
Edit: If helical curve is used (thanks Wolfgang for tip) for pattern, it is easy to achive 17mm shorter pipe then next one.
If pattern is created in assembly using frame component, then every pattern member knows his lenght.
what I tested was, to use a helical curve in a part for a pattern along curve feature to put the components to a circular like pattern with changing height
The bottom face could be created using a boolean substract of a single plane.
If only the resulting body is wanted, then a single part file might be fullfilling the requests.
If You need real parts for every instance then You can use this construction part as input for the edges of a struct frame in an assembly
To show it better, I have used less then the 70 instances for the pattern.
This also depends on You original dimensions
fine to hear.
So, a single part works for You too?
And, be carefull with the helical curve (maybe ST9 issue)
As You can see in the video, I used a 0.5 wind but the result goes over the 180 degrees.
Maybe someone else can confirm that as a ST9 bug or as a Works-As-Designed issue
and it also is no problem to bring it into a structure frame assembly.
You can create a single 3D sketch line within Your part, You can pattern that in the same way as the body and You can use the split curve function to split those curves with the reference plane
And now, you can use those splitted curves with a field selection for the edges of the strucvture frames
I'm astonished and glad about that solution by myself, what man can do using Solid Edge
Going this way You even will get separate part documents for every single component together with the full info about length, weight etc.
I suppose you can also use a body pattern to obtain a multibody part you can publish if you need different parts.
Another solution I was thinking of is to use occurrence properties (you have the coordinate of the parts here) and assembly feature cutout. I saw a workflow using that to obtain some kind of helical pattern before we had it. The downside is that it is not a pattern anymore and you don't really have one file for each part (assembly feature) :
1. do the pattern of the part
2. Break the pattern
3. Go into occurrence properties
4. Use a temporary excel sheet to have a column of +13mm increment (0 , 13 , 26... you have the idea)
5. Copy past in the occurrence properties to position correctly all your instance
6. Then do an assembly feature cutout
Always good to have different solutions
the question might be, how to pattern a single body within a part file and create multiple bodies automatically.
Since IMHO the pattern belong to the current body.
And it seems to be fair an effort to split them into seperate bodies