I am doing some lattice structures using Face Curves, and since it generates Splines SW cannot create Weldments with them.
So I created a lot of Sweeps, but it's a lot of manual process depending on the structure and I would like to lets say, at least be able to change the diameters all together.
- Is there a way to do it?
- Is there a reason why Weldments cannot recognize Splines?
- Suggestions of workflows are welcome
I can not open your file but would like to know as why you created 12 sweep features for the rings? You could have done them all in one single sweep by creating the multiple contours in the same sketch for the profile.
I think the way it is it's not possible to select multiple contours, I created it out from a piece of surface, then patterned the bodies.
Also not possible to do it with the hole ring:
It is possible to do with just one Revolve and one Sweep tho. I used Segments on the Equation Driven Curve sketch and drew the circles with the points, then Revolved it:
But this does not solve the trouble to work with the Splines generated from Face Curves
I would have done this with a single revolve with multiple profiles, and then a single sweep, and patterned the sweep.
As for the weldment/spline thing, weldments are really intended for structural members, which are tough to bend into spline shapes. Even for tube bending, most benders will give you sections of constant radius.
matt wrote: ↑Fri Aug 20, 2021 11:24 am
As for the weldment/spline thing, weldments are really intended for structural members, which are tough to bend into spline shapes. Even for tube bending, most benders will give you sections of constant radius.
I think the new whatever-they-call-it that's supposed to replace traditional weldments will work with splines, but I'm not sure.
"On the days when I keep my gratitude higher than my expectations, well, I have really good days."
Lucas wrote: ↑Thu Aug 19, 2021 10:01 pm
I am doing some lattice structures using Face Curves, and since it generates Splines SW cannot create Weldments with them.
So I created a lot of Sweeps, but it's a lot of manual process depending on the structure and I would like to lets say, at least be able to change the diameters all together.
- Is there a way to do it?
- Is there a reason why Weldments cannot recognize Splines?
- Suggestions of workflows are welcome
image.png
If all the diameters are defined by a dimension just make all the dimensions equal to each other. Change the one that they are equal to and they all change.
Thank you for the answers. One problem a little different: this one does not has a pattern and was done with Face Curves and Sweeps (with Circular Profile). Is there a way to get all the diameters values from the Sweeps and attach to a sheet or something so I could change them together? Instead of just go clicking and changing one by one.
Weldments is a convenient way to do lattices for additive manufacturing, would be nice to have some updates with that in mind.
For the first model it is possible to do another sketch and draw all the profile circles - but not in this situation.
@Glenn Schroeder you mean the new SW online? (3DExperience cloud-based whatever? I don't understand the products mix DS is creating lol)
Lucas wrote: ↑Fri Aug 20, 2021 8:24 pm
Thank you for the answers. One problem a little different: this one does not has a pattern and was done with Face Curves and Sweeps (with Circular Profile). Is there a way to get all the diameters values from the Sweeps and attach to a sheet or something so I could change them together? Instead of just go clicking and changing one by one.
Use a global variable. Use the "circular profile" option in the sweep, and set the diameter of the profile. Then set the diameter to a global variable. I used "d".
Then make other sweeps and set the diameters to "d".
matt wrote: ↑Sat Aug 21, 2021 9:56 am
Use a global variable. Use the "circular profile" option in the sweep, and set the diameter of the profile. Then set the diameter to a global variable. I used "d".
gupta9665 wrote: ↑Mon Aug 23, 2021 2:48 am
Other option is link value using which you can link all the dimensions and then changing any one will change rest of them.
@Glenn Schroeder is correct the spline functionality was added to Structure Systems and not Weldments. DS has abandoned development of Weldments because SS is supposed to replace it...I tried it a while back and it was missing functionality. I keep asking when it will be ready for use; but can't get a clear answer. So, even though it'll do splines it's likely to burn you in some unforseen way after you've sunk many hours into it. So, I'd avoid SS for now.
Another option I haven't seen listed is to use Blocks. You can create a Block with a circle (or any shape) drop it into multiple sketches and use it to drive the profiles. Then if you change the block all instances will update.
Lucas wrote: ↑Fri Aug 20, 2021 8:24 pm
@Glenn Schroeder you mean the new SW online? (3DExperience cloud-based whatever? I don't understand the products mix DS is creating lol)
Lucas wrote: ↑Fri Aug 20, 2021 8:24 pm
Thank you for the answers. One problem a little different: this one does not has a pattern and was done with Face Curves and Sweeps (with Circular Profile). Is there a way to get all the diameters values from the Sweeps and attach to a sheet or something so I could change them together? Instead of just go clicking and changing one by one.
Weldments is a convenient way to do lattices for additive manufacturing, would be nice to have some updates with that in mind.
image.png
For the first model it is possible to do another sketch and draw all the profile circles - but not in this situation.
image.png
@Glenn Schroeder you mean the new SW online? (3DExperience cloud-based whatever? I don't understand the products mix DS is creating lol)
mattpeneguy wrote: ↑Mon Aug 23, 2021 8:21 am
@Glenn Schroeder is correct the spline functionality was added to Structure Systems and not Weldments. DS has abandoned development of Weldments because SS is supposed to replace it...I tried it a while back and it was missing functionality. I keep asking when it will be ready for use; but can't get a clear answer. So, even though it'll do splines it's likely to burn you in some unforseen way after you've sunk many hours into it. So, I'd avoid SS for now.
Another option I haven't seen listed is to use Blocks. You can create a Block with a circle (or any shape) drop it into multiple sketches and use it to drive the profiles. Then if you change the block all instances will update.
I actually don't mind that they've stopped with development on weldments. That's one of the few areas of the software that I can't think of any big thing they could do to improve it (at least for what I use it for).
The inability to use cut list properties in BOM's, or to link to them in title block notes, is one issue that could use some help, but I doubt very much that they'll fix that with Structure Systems either, and there are other things that frustrate me much more than that issue.
"On the days when I keep my gratitude higher than my expectations, well, I have really good days."
Oh, I was doing lattice with Structural Members and totally missed Structure System. lol
Looks like a more convenient way to do lattice, thank you guys
mattpeneguy wrote: ↑Mon Aug 23, 2021 8:21 am
Another option I haven't seen listed is to use Blocks. You can create a Block with a circle (or any shape) drop it into multiple sketches and use it to drive the profiles. Then if you change the block all instances will update.
I will give a try, thanks
Ry-guy wrote: ↑Mon Aug 23, 2021 12:34 pm
Use DriveWorks!
curve cut3.SLDPRT
