So I’ve had a seat of Zw3d since about 2018, but it’s been gathering dust as I could never figure out a good workflow for skeleton / master modelling in Zw3d which I use for about 99% of my models.
Basically I want to have a single part that is a bunch of sketches, planes and surfaces that define my model. I want to then be able to feed this into the subsequent parts to detail up. Call it a skeleton model, master model or Layout model…
In Solidworks I would use the insert part feature to insert the master into all my parts. It’s been a while since I used NX, but from memory i was also able to do this. I think through the wavelink functions.
I’ve just downloaded Zw3d 2022 to take another look at, and found that the “External Part” feature now has the ability to bring all the sketches from a part into a new part, which is a huge help. however it doesn’t bring in any datum’s and I don’t have the ability to see a list of the external parts sketches in the feature tree. This makes it hard to find what I need in larger parts that contain lots of sketches.
Is there a way to also bring in the datum’s from this external part into the new one?.
The reference link features seem similar to NX Wavelink, however I can’t do what I need with this type of linking either as I don’t have the ability to bring whole sketches in, only curves, and all of them only work in the context of an assembly.
Does anyone know how to do this type of modelling in Zw3d?
Can you attach your case?
Are you using soldered modules for the frame?
No i’m not talking about frames or weldments, I’m talking about any part really.
I just want to be able to copy 4 types of data from 1 part to another.
currently I can’t find a good way to do this.
"External part" tool:
this feature functions exactly how i want it to, but is missing the ability to link planes from Part A to Part B.
"Geometry to part" tool
can do all 4 types, but any new data added to part A wont be automatically copied to part B, you have to manually link the new geometry to part B. this isn’t good for large assemblies where lots of parts reference part A as it would quickly become very time consuming.
Only works in the context of an assembly, but cannot link sketches, only curves.
each of these 3 tools work slightly differently, which is great, but why cant I link planes with the external part tool, or sketches with the reference tool?
2023 will be released in a few days, and this one will be improved!
there are assembly references. Once upon a time they where in an Assembly Tab available during part creating in an assembly context. But for some strange reason that tab is not available in 2022. Go figure!
But they are there via Insert in top menu. whilst in a part within and assembly.
This allows you to reference Curve, Datum, Face and Shape from any OTHER object in the assembly.
If associative(default), the reference objects will update whenever you change the parent object and regen all.
What is cool is that these references can be used directly as shape components within the part. and outside of the assembly. e.g. open the part only.
Regards, sketches, use sketch Blocks created whilst in the assembly.
Then you can reuse the Block as many times as you like in other parts in the assembly.
IMO - Skeletal Design is perhaps a bit complicated and unless you have a specific application that works/needs it. 2D type assemblies seem to be the best candidates.
I did a stair way model that was one parent sketch that had lots of calcs to design the various component dimensions. Then each dimension was named and used to drive(expression) the part development within an assembly.
The sketch was visible within the assembly so you could see when everything was correct.
The sketch was the design check and the easy place to develop the correct dimensions for everything.
It was easy to copy the complete assembly (Multiobject file) and make many variants or stack the stairs for multi level development.
It took a while to do it and was worth effort since that was repeated over and over again.
I am not sure how it would be done in a SO environments since name management becomes a problem or if it would be worth if for a one off design.
FYI - there is a post devoted to this subject.
So my question to you is - even though you have designed that way before, is it the easy way in ZW?
Cheer - Paul
I’ve just downloaded the 2023 installer that you linked in the other thread.
I assume you were talking about the “publish set” tool?. having a 10 second play with that and the “copy all valid from pick file” in “external geom copy” tool I have to say this is 100% what I’ve been needing since I 1st started using zw3d back in 2018.
This is brilliant!. I think i just put solidworks in the bin.
thanks for your detailed reply.
I saw your thread on expression driven assembly, and I agree it’s a great way of defining certain types of projects, but in nearly 20 years of cad, it’s not something that I’ve ever had a project that could utilize that type of approach. The industry I work in just doesn’t tend to do that sort of work. I’m definitely glad Zw3d can facilitate it though should I need it.
As I replied to Liangfen, 2023 has all the tools I need now to link larger amounts of data in an automated way, which is fantastic. I think this version will allow anyone from my industry to use ZW in an efficient and familar way, which is always a good thing
This is good news
This version of the variable browser has changed a lot, and the system also has an option to control whether it is valid externally.
I haven’t seen 2023 yet or even a Whats New.
I’m a bit challenged downloading large files for the moment and ZW have not done a great job of previewing 2023 online.
What type of items are you modelling?
Cheer - Paul.
Do you use Assembly reference tools already?
If so, to what extent?
I have just read up on Skeletal Modelling.
It seems to me that whilst there is no Treehouse or special model, the tools are there but in a mildly different way.
I am curious how many other use Assembly Reference tools or alternative don’t know how to use them?
Cheer - Paul
Our forum doesn’t seem to support uploading PDF directly。
Hi Liangfen, try now.
Cheers - Paul
FYI. the Forum is in a container so it has limited resources but these resources are guaranteed. A plus and a minus.
If a PDF is publicly available then a link should be posted. If it is a privately developed PDF that is being shared then upload is OK as long as it is relevant.
In a tidy up of resources, it might be discarded if the use is low.
Cheers - Paul
That’s good news!
My resseller have a Whats New page:
Thank you Paul.
I was not aware of this command ( I don’t remember having see it in the documentation pdfs I read) , and I had lots of lost geometry problems in my assemblies.
I think it will solve some issues I got, and perhaps all of them