Working and managing your surface model in SW?

[osdecar]

Hi Everyone,

I am trying to learn SW after several years using Catia.
Solid modelling seems to be pretty similar across most CAD packages, but surface modelling is a completely different thing, and I am totally lost in how to do things in SW. I'd like to ask you a couple of questions, and maybe you'll be able to show me what's the best way of working with SW for those cases.

• Question 1: Re-using surfaces for several different operations.

It seems like the logic SW uses for surfaces is very similar than for solids, with this linear timeline that goes in one direction. So once you have used a surface for one operation, then that surface cannot be used somewhere else. This seems to me an extremely rigid logic that makes modelling quite difficult and frustrating. Am I right or maybe there's another way of working in SW?
For context, in Catia, you can use the same surface over and over in several different operations, leading to several different children. In the same way you can use the same plane to create several sketches, or the same point to create several lines.

So, in my attempt, the final geometry I want to achieve looks like this:


The main thing I wanted to test here was the shape of the ribs, and how to trim them. So I approach this in the following way:


I created surface1, surface2 and fillet them together:



Then I gave it thickness and created the ribs:



I created an offset of Surface1. But I couldn't use surface2 to create another fillet, because it was already used to create another entity. So I couldn't trim the ribs to the desired shape.



I finally found a workaround by creating a 0mm offset of surface2.


Then I used that fillet to trim the ribs as per the picture above:

• Question 2: Replace elements (so all the children of the replaced one, are now updated to the new one):

Imagine in my previous example, I had drafted all the faces to the die line (dotted blue), and now, for whatever reason I want to change my tooling line to a different one (solid, orange). Is there any way to do this replacement in one single operation? Or do I have to manually change ALL the drafted profiles and surfaces to refer to the new die line?





If you've reached this far, thanks for sticking with me. I understand I might be trying to work like Catia in SW, that's why I'm trying to understand what's SW best way of working. It's very frustrating that all the tutorials out there, even books or paid courses are aimed at showing how the commands work, but not so many are focused in how to actually work with the software.

Thanks everyone

[AlexB]

In my opinion, surfacing doesn't make much sense until it does.

1. There are workarounds like you've found to use the same surface multiple times (Offset 0mm) since surfaces are often consumed to create a child feature.

2. This might be easier to answer if you were to post your example model. In my experience, it is possible but the design intent to have the draft direction be flexible needs to be set up early in the feature tree. Going back to change draft direction if it's not been set up that way can be cumbersome.

[osdecar]

2. This might be easier to answer if you were to post your example model. In my experience, it is possible but the design intent to have the draft direction be flexible needs to be set up early in the feature tree. Going back to change draft direction if it's not been set up that way can be cumbersome.

I can upload my model, but I don't think any specific solution to the particular example would be applicable to the generic problem.

-What if I had made several sketches in "top plane" and later in the design I realised I wanted to use an slightly tilted plane.

-What if I have a flat top surface and then I wanted to change it to a curved one.


I think I'm too used to this kind of flexibility that you can have in Catia, that I'll struggle to adopt SW



EDIT:

I have casually found this video explaining the differences between "Standard geometrical Sets" and "Ordered Geometrical Sets" in Catia.

Looks like SW uses the same logic as the "ordered geometrical set". Is there any way to change to the other type of logic? Or this is the only way of working in SW?

[bnemec]

I can upload my model, but I don't think any specific solution to the particular example would be applicable to the generic problem.

-What if I had made several sketches in "top plane" and later in the design I realised I wanted to use an slightly tilted plane.

-What if I have a flat top surface and then I wanted to change it to a curved one.


I think I'm too used to this kind of flexibility that you can have in Catia, that I'll struggle to adopt SW



EDIT:

I have casually found this video explaining the differences between "Standard geometrical Sets" and "Ordered Geometrical Sets" in Catia.

Looks like SW works with the same logic as the "ordered geometrical set". Is there any way to change to the other type of logic? Or am I stuck with this way of working?

Yes, in ordered mode it's like a computer program, most things are hinged on what you've already done. So you can either continue forging ahead using cuts and extrudes and direct editing to make changes, or you embrace history-based modeling and go back in time to edit the past. Do this for a while and you will learn how to model parts in history-based modeling so that they can be edited in the future.

"-What if I had made several sketches in "top plane" and later in the design I realised I wanted to use an slightly tilted plane."
- if your sketch was done with care and not willy nilly sketch relations and dimensions you can simply go back in time to before the sketch, create a new plane at whatever angle you like, edit the sketch to use the new plane. I suggest you make your new plane based on the top plane for sake of not flipping normal or yawing 90 degrees. A few things will need fixed in the sketch. If everything in the sketch blows up and you don't see how you could have constrained it better, then I suggest Solid Edge Sycn Tech.


-What if I have a flat top surface and then I wanted to change it to a curved one.
agreed, this one is probably better done in better systems. There's some features in SW that supposedly make this "Seamless" and "simple" like Dome maybe but I don't know about that. I haven't used SW enough but in SE this can be a good place to use a surface then replace face. The "Blue Surf" in Solid Edge isn't too bad; otherwise some type of lofted surface. If surface and replace face doesn't work nice then I'd go to creating a new body that just defines the new curved face and then Boolean add them.

[Arthur NY]

So going to list quite a few things that I'm hoping will help you wrap your head around SW Surfacing capability.

First from a resources point of view it really doesn't get much better than Matt L. If you're able to find either the physical or digital version of the "Solidworks Surfacing Bible", even though it's was released about 10+ years ago a lot of the base functionality and overall modeling approaches are still valid. Matt also has an online surfacing workshop...(https://episodes.dezignstuff.com/blog/membership-join).

GrabCad…. Is filled with 1000’s of models and a good majority of them are Solidworks models. Now some people don’t know how to upload an Assembly properly because they forget to also upload the associated Part files which can always easily be done using Pack and Go….that aside, even if you’re not 100% interested in a design, one of the biggest upsides to history based modeling is that you get all of the ingredients as well as the receipt and how they the meal was made. Rolling back the history of a model to see how each feature is used can give some amazing insight as to some of the how and why. I do caution that just because a model is uploaded that the person that made it may not be as 100% optimized as possible. It can be challenging to do that every single time on every single project.

Dimonte Group….(https://dimontegroup.com/news-resources/) If you haven’t looked them up then you’re missing out on some of the most robust Solidworks specific modeling tutorials out. Ed Eaton and Andrew Lowe have done amazing presentations over the years that will keep you busy for the next 6 months.

That said, the great thing about history based modeling is that there is a domino effect and things are quite linear. The "Bad/Challenging" thing about history based modeling is that it's challenging to be flexible midstream when drastic changes are needed. This is definitely a subjective term and can have several meanings depending on who you ask and in what software is being used. Some of what you’ve encountered are indeed workarounds not every feature is absorbed by the
operation….. This is the tricky part, knowing which features do and which ones don't is just something that comes with time and using the software.

With what you’ve described about changing from the Top plane to an angled plane that’s easy. Switching to any type of curved surface is just setting things up for potential failure if trying to sketch on directly. This is an area where things can really go wrong if not paying the utmost attention to what’s happening. There is a big difference between the 2D and 3D sketch solver and even when trying to button things down in the 3D sketcher its voodoo magic at best. You would do better projecting onto the curved surface from a 2D sketch but again this is very situational.

While Solidworks does not have the two distinct possibilities shown in the video, there are slight possibilities to work in this manner using the rollback bar. In this way there are ways to add in new sketches or features into the middle of a model BUT when going this route nothing after it will know that it’s there. In other words you’d have to point any feature below the rollback bar to the new items that have been placed into the middle of the history.

There’s probably much more that could be unpacked here but this is a ton of info to begin to sort through and digest. Hope this at least helps.

[zxys001]

you can always copy surfaces from the original to add into your othe operations.