I have a frame drawn up and need the weldment tube profiles to change based on the size of the frame. Is it possible to do that using equations instead of manually selecting my profile every time?
You can do this easily if the same sketch will suffice.
Just adjust the sketch dimensions directly by equation.
Add configurations if you need.
To make sure the description and other cutlist properties still make sense you can link the dimensions to the properties.
I could show you an example tomorrow if you have any questions.
Sorry for the late replay. Could you show me an example of what that my look like?
Henry Wall wrote: Sorry for the late replay. Could you show me an example of what that my look like?
Henry Wall wrote:
Sorry I don't have time at the moment to give a thorough run through - and this example might be a bit confusing.
but the takeaway here is that you can link 'any' cutlist property to a sketch dimension from the weldment profile sketch itself and then change the dimension however you like.
This example is a bit confusing because I am also using a configured profile.. but we only use the configurations to provide a 'text description'
You can take this as far as you like.. for example we have a long description that brings in the Description, Length, Width and Thickness. - and these last 3 dimensions can be controlled directly by equations and update correctly in the cutlist
For this to be automatic, this does mean setting up your weldment profiles..
It's a trick I learnt from Deepak here Frustration with cutom weldment profiles
We don't really use weldments so much anymore, preferring to go down the assembly route, but it served us well for a good few years.
Rob Edwards has a great suggestion.
But, depending on what you are doing DriveworksXpress may be the perfect thing for this. Or, a design table could be used to drive the dimensions. It is really hard to know without more information.
Can you post some screenshots or parts/asms/drawings? If there's intellectual property involved, maybe you could explain the situation a little more.
You can do this with [without] configs and [instead use] feature suppression in the equations dialog.
Create structural members from the same sketch and suppress them.
Create global variables that evaluate to zero when the config is required and 1 when it's not.
In the Features section, pick each structural member from the tree and select its associated global variable.
Since the length is 18, the L angle frame is suppressed and the pipe frame unsuppressed:
Set the length to 28 and the pipe frame is suppressed and the L angle frame is unsuppressed:
EDIT: I initially meant to say "without configs" as this will maintain the as machined, etc configs, but I didn't type that correctly.
Edits in  above.
Feature suppression is a good way of doing this. With my situation though, i have all square and rectangular tubing. All i would need them to do is change sizes based of certain widths and heights of the frame.
Henry Wall wrote: Feature suppression is a good way of doing this. With my situation though, i have all square and rectangular tubing. All i would need them to do is change sizes based of certain widths and heights of the frame.
I just did this quick picking different profiles, but it's the same thing for profiles of the same cross section.
Just create a new structural member based on the same sketch. It can be in the same profile family but of a different size or from a different profile family (as I first posted).
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