Creating a compontent pattern from a fill pattern?

[StefanHamminga]

Current situation:

I have a part with a cirular fill pattern, 3mm holes.
In these holes I want to place tubes. The first is allready shown.
SolidWorks won't let me use a feature driven component pattern (I get a message I can't use a fill pattern for my feature driven component pattern).

Besides mating each tube indepenently is there any other way? Tubes are to be of a different material.

The assembly:

The tube:

Stefan Hamminga
EngIT Solutions
CSWP/Mechanical designer

 

[Bouke]

How about creating a sketch in the part with the holes with only dots in the centers of each hole and then use sketch-driven pattern?

Bouke Brouwers
M-Des
The Netherlands.

 

[SBaugh]

The only thing that I can think of would to be make the tube part in the part level and make it a Separate body and use the same fill pattern command and place that component into your assembly.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376

 

[CorBlimeyLimey]

... or mate a tube in one hole of each circle of holes and then do a circular pattern of each tube?

... or create as a multi-body part and then Split and Save-as individual parts?

An ER for a Fill Pattern to be used as a feature driven component pattern would be good.

 

[StefanHamminga]

Bouke, creating the sketch points is quite a bit of work by itself, with 300+ points to go. I'd prefer a solution that is parametric as wel (as in, updates according to changes in the pattern).

Scott, that seems to be the best solution. I had thought of that as well, using weldments. disadvantage: manual updating of the BOM is needed.

Cor, the tube circular patterns could work, but it still is pretty labour intensive. The multibody & save as assembly method creates a part file for each seperate body, not able to use multiple instances of the same body in a newly created body. Quite stupid actually, since the weldment feature is able to recognize identical bodies.

I'll fill in an ER for both.



Stefan Hamminga
EngIT Solutions
CSWP/Mechanical designer
Searching Eng-Tips forums

 

[Bouke]

Just a quick thingy that came to mind.

The pattern you used to create the holes in the original part could probably also been done in the sketch lvl instead of making a feature pattern.

So, you could create a sketch containing only points of the entire pattern, which should be just as much work as creating the feature pattern of the holes. Then use that sketch for a sketch-pattern where you pattern the cut-extrude feature. That should add only 1 extra feature in your part which is not time-consuming.

Now in the assembly you've still got this sketch anyway to use to pattern the tube.

Then as result you would have your parametic solution right?

Regards,

Bouke

Bouke Brouwers
M-Des
The Netherlands.

 

[CorBlimeyLimey]

Unfortunately the Fill Pattern only works for features, not sketch entities.