So I have been messing around with Design Tables in Solidworks 2019. I am new to using these, and was curious about something.
Something to keep in mind here is that a finished good we produce has more than 1 component. Typically we have 3 - 8 components in each part. And each component is drawn in a single model, using different sketches (if that makes sense). I do not model each component individually and bring them into an assembly.
Since there is a way to have a model automatically updated to named dimensions used in a design table, is there a way to have a drawing automatically populate dimensions based on model dimensions?
Instead of having to manually pull in the model view, sectioning it, and re-applying every dimension, is there a way to have it do that automatically?
I'm sure this is possible, I just have to deep-dive into how formulas or macros work etc... just looking for some direction on this, not for someone to do it for me.
Any direction on this would be greatly appreciated!
Thanks!
Can you post some screen shots or some files? You can do a lot with Custom Properties and Design Tables. I'm sure you can get to where you need to be, I'm just not 100% on what you are trying to do.
As to one of your questions, I think you can just have the dimensions you want to appear come into the drawing by default if you changed this in your drawing template:
I will try my best to explain with screenshots, without too much information.
So we manufacture PTFE rotary lip seals, and we make each component for the seal, in house.
We have certain standards that we follow for dimensions of each component.
Here is a picture of a basic final assembly:
Components are labeled as follows: A - Outer case
C - Gasket
E - Sealing Element
B - Inner case
So my questions, is there a way to pull in dimensions for an outer case manufacturing print (for example):
The above image is the dimensions of the outer case for the final assembly. Just for the model. Not all of these dimensions are needed for the manufacturing print, as we make these cases on a manual lathe / press by spin forming the metal on lathe, and punching the center hole on a press. NOTE: This picture is of the finished part, of an assembly.
The following picture is of the same outer case, but for manufacturing:
The above picture is a basic manufacturing print template that I've created. As you can see, we make the case roughly .060" longer in length than the finished assembly, to allow for some material to bend over and compress the inners of the seal.
So I'm wondering if I am able to somehow make a model of the finished assembly, then pull in dimensions onto a manufacturing print for each component, with some dimensions being different than the final assembly.
I hope this all made sense lol I'm not the greatest at asking for help and knowing how to ask properly.
Thanks in advance!
Go into the sketch you show uncheck any dimensions you don't want to show in your drawing by toggling this off:
Then make sure it's toggled on for the dimensions you do want to show. Then when you create your drawing only the dimensions you want to show will show up when you bring in model dimensions:
Do similar all the time for welding.
Use config in part and assembly.
Part need a "Flat" for laser/plasma/waterjet with machine allowance.
A "PreMachined" for premachining before weld.
Sometime a "Machined" for machining after weld. Yes, I may not put "machining" in assembly.
Assembly will have similar config for each step.
Sometime Display State is used.
In drawing, select the config/display state required.
Ok I think I kind of get what you're saying. I've created configurations for each component, inside the final part file, to show manufacturing dimensions. So would I need separate design tables for each configuration? Or can you have 1 design table file that controls every configuration?
I think you don't need design table.
You can select the config in drawing view.
I was using the design table because we design many many different sizes of these seals. So instead of having to go in and adjust multiple dimensions separately in the model to make it the correct size, or remodel from scratch. I figured it'd be nice to use a design table, edit the dimensions in the table and pull it into the model template to auto-model.
For that style seal that I sent pictures of, we make seals from shaft size of Ø.125" up to shaft size of Ø31.496". And bore sizes ranging from Ø.566" up to Ø33.479". So that's where I figured design tables would make that easier. Most customers ask for a .STEP file to fit the seal we make for them into their assembly of their application, whatever that may be.
Design tables are definitely a good tool for this. I don't use it, but there's also DriveworksXpress. It comes free with SW. You should definitely look into how it works, it may be perfect for your workflow. You may even want to get the full version of that software from your description.
After looking into, and experimenting with DriveWorksXpress, I definitely have some studying to do. Lol This is new to me, and I am lost as to how to set up the rules properly. Some homework for sure
I haven't watched it, but this may be good:
Lunch & Learn - DriveworksXpress - YouTube
I don't like linking to youtube videos generally because there are a lot of bad ones. But, if you can find the ones put out by the VARs, they're generally pretty good. So, ones from Javelin, Hawkridge, MLC-Cad, Trimeric, etc. should be good. Also there are a bunch by DriveWorks, and that's the company that makes the add-in. So, their videos should be good too.
There is a tutorial and test for cert in Drivework website.
I got the cert, it was painful.
Awesome Frederick!
Kyle,
I'd start here DriveWorksXpress Training & Certification - How To Videos - YouTube
So I have completed one Project for one style of seal we manufacture. And I have it all correct, automatically pulls model / dimensions into a print template for manufacturing.
Only question is, is there a way to set an automatic scale somehow, so for example if I run the Project for a 2 inch Ø part, and then a 9 inch Ø part, they pull into the drawings the same just with new dimensions?
To add to my previous comment:
I ran some test parts through it to see the capability, and when I made a larger diameter part, the scale was all messed up and I had to readjust it to fit the print properly.
Any fix on this?
You might need a macro in the drawing to do that.
Yay, more homework. lol I'm terrible with macros
Get detail of what you want.
Start a new post in API/Marco.
Ask nicely and someone might write you a macro.
Me too...We can't all be Artem Taturevich or Josh Brady...But the really great thing is if ya can't figure it out, they're often there to give us a little help. So, when you get a chance post your attempt over in the API/Macro area.
I'm on it. Thanks for the advice, Matt! I appreciate your guidance!
Can you change config for the view?
I'm sure some In context modeling could be useful here instead of driveworks. Set up values in an Assembly equation manager and apply them to the dimensions of the parts?
By having the values controlled from the assembly, the dimensions should update itself on the print and then figure out the scaling problem from there
Good point Jason Martin.
Kyle Litwin,
Are you familiar with the SSP method? https://forum.solidworks.com/search.jspa?q=SSP