Mirror a pattern in a weldment. 1

[eworden]

What I'm trying to do seems simple, but I can't seem to get satisfactory results.

Goal:
I have a weldment with a pattern of structural members. The weldment is driven by a design table.
The tubes are evenly spaced at 48", I want the structural member to be symmetrical. When I increase and decrease the overall size, I want the pattern to change proportionally and remain symmetrical to the center line of the weldment.

My attempted method:
[ol 1]
Create structural member along center-line of part.
[/ol]
[ol 1]
Pattern structural member in one direction, with pattern driven by equation(total width/48 = pattern number)
[/ol]
[ol 1]
Mirror structural members across plane on center-line.
[/ol]

Problem:
When I increase my size in the design table, the mirror feature does not include the new structural members created by the pattern feature.

This sounds like the solution I'm looking for:

To mirror a pattern on multibody parts:

[ol a]
Under Features to Mirror , select the pattern from the FeatureManager design tree.
[/ol]
[ol a]
Under Options, select Geometry pattern.
[/ol]
[ol a]
Under Feature Scope, specify which bodies you want the feature to affect.
[/ol]

However, when I try this, it will not allow me to select the pattern. I get no error message or anything, it just does not allow me to select the pattern at all.

Am I misinterpreting the instructions? Is this not available in weldments? Is there some other way to accomplish my goal?

 

[Gupta65]

I believe that it might be a limitation while working with Weldment but yes it can be a nice enhancement.

As a workaround, you can create another pattern in the other direction and link the dimensions to the dimension of first linear pattern. I just tried it on an example file and it worked.



Deepak Gupta
CSWE, CSWP, CSDA
SW 2011 SP5.0 & 2012 SP3.0
Boxer's SolidWorks™ Blog

 

[Jboggs]

A weldment is a multibody part. When you are using tools like mirroring or patterning in a weldment you should always mirror BODIES not FEATURES. In our experience here that has been the most common problem encountered in weldments. I'm not saying you don't understand this. I'm just saying many designers where I work do not. It makes sense when you think about it. When you weld a new component to a frame you aren't "adding a feature", you're "adding a body".

Unfortunately when you select a MIRROR or PATTERN tool, Solidworks assumes you want to mirror a feature and sometimes even automatically fills in the feature field. When it does that erase the selected feature. Highlight the BODIES field, and select the bodies from the display rather than the feature tree.

 

[JMirisola]

When you mirror weldment features, you're mirroring the bodies not the feature. Because you have to select the bodies individually, after the linear pattern is changed, you'd need to select the new bodies.

Jeff Mirisola
Director of Engineering
M9 Defense
My Blog

 

[eworden]

Thanks for you responses!

I understand how to mirror individual bodies. That is currently how my part is set up.
The only problem with that method is that when I update my part and my pattern increases, the new bodies created by that pattern are not included in the mirror feature. The work-around is, every time I change my configuration I need to remember to manually go into the mirror feature and select all the bodies I want patterned. This undermines my goal of making a parametric driven part.

Lets take weldment out of the equation.

I made a simple multi-body part:
1. Extrude boss
2. pattern boss disjointed
3. mirror all bodies

Is there anyway to change the instances patterned, and have those changes automatically reflected in the mirror feature?

 

[Jboggs]

If I understand your question, you are trying to set up configurations that differ in the NUMBER of instances in a pattern. Right?

If so, think outside your box. Set up the pattern in the basic part with the maximum number of instances that will be required in any configuration. That pattern will probably extend well beyond your basic part. The next step is to set up an EXTRUDE CUT feature that applies to ALL BODIES. The sketch for that extrude can be anchored at one end on the last pattern instance. The other end of the sketch is anchored to some point determined by your configuration. Basically you are creating all the bodies you will ever need, and then erasing the ones you don't need for that configuration.

Could work. Let us know.

 

[mjcole]

You can try using the Pattern Seed Only Checkbox to only pattern the Original Body used for Pattern in the second direction. It is there for exactly this type of case.

This will prevent you from getting P1 * P2 5X5=25 Instead you'll just get (P1+P2-1) or 9 Instances.

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