CAD Forum

I though I would drop this here for people to review.
It's a document that I've compiled over several years that I give to new coworkers as a guide
Keep in mind, some of the techniques/examples are company specific.
I hope I pulled out everything company specific.
Our company build case good so mostly wood panels.
We outsource our form metal.

Looking for critique and input.

Bryan O wrote: ↑Thu Oct 31, 2024 3:43 pm Looking for critique and input.

TLDR. Can't you just spoon feed these to me as I need them?

Honestly though, pretty good list. About a 1/3 of it applies to our use case and I think are nearly universal. Some of it is use case specific; ex. using mirrored configurations and parts are always specific to assembly. We almost never have more than one part number per file. Which also means welded parts are assembly files.

In addition to always hiding sketches, also hide all the planes and other reference geometry.

I do have a question about Tips and Tricks 36 Unlink Display States. Is this a universal problem or case specific? I've been linking display state to config on sheet metal parts. It is the only way I've been told to get SW to stop showing bend line sketch in the assemblies (where the model is obviously in the formed state). A real problem when there are a lot of sheet metal parts in upper level assemblies and need to view a sketch.

bnemec wrote: ↑Thu Oct 31, 2024 4:59 pm I do have a question about Tips and Tricks 36 Unlink Display States. Is this a universal problem or case specific? I've been linking display state to config on sheet metal parts. It is the only way I've been told to get SW to stop showing bend line sketch in the assemblies (where the model is obviously in the formed state). A real problem when there are a lot of sheet metal parts in upper level assemblies and need to view a sketch.

I don't have any issue with bend lines showing whether display states are linked or not. We always hide them and usually we have displayed states unlinked.

Bryan O wrote: ↑Thu Oct 31, 2024 3:43 pm I thought I would drop this here for people to review.

I like your list. Very Useful. Most things follow our own practices.

I don't quite agree with item k, which says to avoid sketch arrays and use array features. I think sketch arrays are pretty handy and powerful, especially when you use sketch constraints to control them instead of using numbers in the array properties window. Among other advantages, when editing an assembly, you can click on a face and edit the parameters for both the seed features and the array features together.

Dwight

Dwight wrote: ↑Fri Nov 01, 2024 7:59 am I like your list. Very Useful. Most things follow our own practices.

I don't quite agree with item k, which says to avoid sketch arrays and use array features. I think sketch arrays are pretty handy and powerful, especially when you use sketch constraints to control them instead of using numbers in the array properties window. Among other advantages, when editing an assembly, you can click on a face and edit the parameters for both the seed features and the array features together.

Dwight

There are use cases for both, but features are preferable in most ways as they generally become less confusing to the unseasoned users. I have a document very similar that I use as a training tool. I give it out to new employees and give a "reminder" 1 hour over-read with everyone every year. When I get the time, I will definetly look to see and add what is in yours but missing in mine, and if I see anything that is in mine that is not in yours I'll try and share it.

Dwight wrote: ↑Fri Nov 01, 2024 7:59 am I like your list. Very Useful. Most things follow our own practices.

I don't quite agree with item k, which says to avoid sketch arrays and use array features. I think sketch arrays are pretty handy and powerful, especially when you use sketch constraints to control them instead of using numbers in the array properties window. Among other advantages, when editing an assembly, you can click on a face and edit the parameters for both the seed features and the array features together.

Dwight

This.

I think what confuses a lot of people about sketch patterns is that they expect them to be static based on the parameters you enter in the property manager, just like feature patterns are. Once you realize that this is intentional to allow you the flexibility to define how the pattern instances are constrained using additional sketch relations it opens up a lot more options for ways to define your parts.

josh wrote: ↑Fri Nov 01, 2024 8:39 am I think what confuses a lot of people about sketch patterns is that they expect them to be static based on the parameters you enter in the property manager . . .

Well put. I think that is the case.

I also struggled with the fact that what it calls the X-Axis, is not the global part X-Axis.

Thanks for the input! Keep it coming!
@bnemec We generally don't use display states and (I might be wrong) but I was told they are a memory hog.
@Dwight I'll have to look more at sketch patterning. Maybe I haven't looked closely at it enough.
@AlexLachance The end goal of this is to get as many people using the same techniques as possible.
I have a few coworkers who overthink things and try to outthink the software. Then there is also the flipside, the "lazy modeler".
My basic premises is KISS and model so someone following you can understand what is going on.

Bryan

I thought display states are better than configurations or sections for performance. I'd like to learn if that's not the case.

There's a thread I started on sketch arrays with a link to a video at https://www.cadforum.net/viewtopic.php? ... ray#p20054.

Dwight

I like your list... it mostly follows the best practices mantra I promote in most ways! Good job!

Thanks @Dwight ! I appreciate the video.
Most of ours parts use configurations for lengths and hole counts.

Attached is an example of how I use Feature Pattern.
"Up to Reference" has been a GAME CHANGER for me!
I can change pattern count (configurable) without having to go back and change sketch geometry.
There is some additional reference geometry but it's simple rectangles.
I can make it symmetrical or not.
1 downside is I have not found a way to "Instances to Skip" that is configurable.

1000 ways to do the same thing, Seeing how others do things always helps me make better choices for our applications.

SPerman wrote: ↑Fri Nov 01, 2024 10:18 am I also struggled with the fact that what it calls the X-Axis, is not the global part X-Axis.

Yah. I struggle with that to.
What I try to instill here is "Model in Real World Orientation"
We make desk. A desk top should be drawn on the TOP plane with the extrusion in the -Y( so the top/middle of the surface is 0,0,0)
I would prefer the top be A sketched witch contain the overall dimensions dimensions (W&D) as these are the most common to change.
This would put the sketch on the XZ plane.
The thickness (Extrude IN -Y) changes far less.

A side panel would be similar: the sketch would be on the YZ with the extrusion being X

When dropping parts into an assembly, orientation does not need to change.
and HOPEFULLY, as most of our part have symmetry, they can be aligned with the assembly planes.

Dwight wrote: ↑Fri Nov 01, 2024 7:45 am I don't have any issue with bend lines showing whether display states are linked or not. We always hide them and usually we have displayed states unlinked.

At the risk of hi-jacking thread, but hopefully it's relevant and points out how use cases affect many things. Hiding the bend lines in the flattened state causes there to be no bend lines in the dxf, which we need. This is the thread that sums up my research and conclusion on flat patterns, configs, formed parts not showing bend lines in assemblies and bend lines showing on dxfs from models.
https://www.cadforum.net/viewtopic.php?t=2471

SPR 754516

Edit: We don't use display states vast majority of the time and never in a part file. I had no idea what linking display state meant. We're just another victim of unused features causing problems by not working together.

Dwight wrote: ↑Fri Nov 01, 2024 12:53 pm I thought display states are better than configurations or sections for performance. I'd like to learn if that's not the case.

To answer my own question, the technical sites believe display states are lighter than configurations:

https://help.solidworks.com/2019/englis ... mblies.htm

"Switching from one configuration to another can slow performance, especially in large assemblies, because the software is loading a different model. Switching from one display state to another can be faster because the model data is already loaded."


https://hawkridgesys.com/blog/overview- ... lay-states

"Utilizing display states allows for the quick transition between these different model appearances. Though colors of a model can be changed between different configurations, as long as the physical model is the same in both it is generally recommended to make appearance changes in display states due to the performance gains."


https://www.javelin-tech.com/blog/2022/ ... gurations/

"Using the display states is much less computationally demanding than having unnecessary configurations."

I assume this advantage applies to the performance of drawing views. We use a display state in a model to hide items in a drawing view in order to reveal hidden items, instead of using a section view or an exploded view. Our top level assembly drawing need all the help they can get.

Dwight

I believe there was also a case study where feature patterns had faster regeneration times then skecth patterns.

TTevolve wrote: ↑Mon Nov 04, 2024 11:32 am I believe there was also a case study where feature patterns had faster regeneration times then skecth patterns.

Can you remember where to find this study?

Just did a test,

Version: SolidWorks 2024 sp5

Feature Pattern:

• Cut Extrude. 0.125 Diameter sketched hole
• Linear Feature Pattern 20 x 100

Sketch Pattern:

• Cut Extrude. 0.125 Diameter sketched hole
• Linear Sketch Pattern 20 x 100

Each time did a Force rebuild (Control Q). Quite a difference in rebuild times. Also of note, working with the sketch pattern results in some selection and highlight delays.

Frank_Oostendorp wrote: ↑Wed Nov 06, 2024 8:50 am Can you remember where to find this study?

https://www.cati.com/blog/picking-apart ... -sketches/

But you can do it yourself as jcapriotti did. There are times to use a sketch pattern, and on small number of copies it's effect is minimal, but on large patterns of holes or shapes it can make a huge difference.

Was wondering how a cloud based CAD system would handle this, Onshape in this case.. The rebuild time for the same part with a 20 x 100 feature pattern rebuilt in a similar time, slightly faster than my 5 years rig (.65 vs .91 secs).

The sketch pattern rebuilt in 7.5 seconds, twice as fast as my rig, although I'd expect similar results with a newer CPU.

Larger patterns were a no go, looks like cap it at 2500 instances. I was able to go to a higher count with the sketch pattern but hit a limit of some sort at 50 x 100. Just wouldn't take a larger number. Increased rebuild to 51 secs, not bad compared to SolidWorks.