Is it possible to turn off the history tree??
Thanks in advance,
FMJ
Printable View
Is it possible to turn off the history tree??
Thanks in advance,
FMJ
You mean to run a history-free feature tree like IronCAD or Fusion360?
Pretty sure you can't do this in Solidworks, there is a reason the programs that offer history-free feature sets have that built in from the ground up. Solidworks is fundamentally a feature/operation history based program.
What is the purpose? There is always a work around (not always a stable one!), even in Solidworks.
I have a SW file of a part I am to machine. I am building a fixture to hold the part by extruding geometry off the part model.
Once I have the fixture designed, I want to delete the part model and just have my fixture without all the errors.
I have started to make an assembly out of the file and I can delete the part model. I then save it as a parasolid and close the assembly without saving.
I get what I need to make the fixture, but it isn't exactly something I want to send back to engineering.
Make the fixture in a part file. Insert the part you want to use as the part model using Insert -> Part. If you need to locate it via constraints, make sure you have the move using constraints option selected at the bottom-ish of the options. You can always edit the part insert feature and check that again to add or redo constraints, so no ctrl-z panic necessary.
Perform all of your edits on the bodies and not on parts in an assembly. When you are doing an extrude to make a new part, uncheck Merge and it will make a new body. When doing cuts, uncheck Auto Select bodies to apply it to and click only the appropriate body. If you hide any other touching body it will autoselect only the one you cut.
This method is called using a Master Model. You will go to the Solid Bodies folder under Annotations in the feature tree and right click the appropriate body and "Insert into New Part". Put ALL form, fit, function, aesthetics features into the bodies in the Master Model. This .sldprt file will serve as your edit ground for form fit or function. Once you Insert Into New Part on all component bodies so they are their own parts, you can do any non-form/fit/function edits needed for manufacturing in that part file. THEN make an assembly and insert each of them. If you just insert at the default location they will be fixed based on the locations they were in the Master Model file. Otherwise float them and apply constraints, motion or static as needed. You can even setup a layout sketch to define complex motion paths and constrain the parts in the assembly to the layout sketch.
Here are two pretty good YT regarding it, though they assume you are working with molded plastic parts rather than mechanical fits, it is exactly the same process. This is the process typically used in Aerospace in complex systems and assemblies, but it is absolutely the most robust and reliable way to build a fully functional assembly that you can edit reliably and will rebuild quickly.
https://www.youtube.com/watch?v=ykj6vTlzYdI
https://www.youtube.com/watch?v=qi4OTvp9yQM
FYI you can also delete bodies from the Solid Bodies folder within a .sldprt file and it will save the body delete in the history, so you can Insert -> Part and then Delete Body on that inserted part body after you no longer need it in the file.
I see what you're trying to do. You want a fixture to be based on a part, but you want to remove the part when you're done designing the fixture. Or something else?
You can also insert a part into a part, if that's helpful. It's not an assembly per se, but it is made up of stuff you bring in from outside, and you can orient it similarly to how you would mate parts in an assembly. And then you can hide the body!
I've done what you're trying to do a thousand times, and I don't think I've ever wanted to delete the model afterward. You know you can turn off visibility, right? What do you think you're going to accomplish by getting rid of the part?
If I could turn off visibility, I wouldn't be posting. When I hide the model, the fixture goes with it. Thanks for your help.
It seems that you aren't separating the fixture and part model. If they are being done within the same part file, make sure you don't merge them via an extrude or revolve with "Merge" selected. This way they will be separate bodies and you can hide (or delete) the part body.
That, or make part and the fixture separate parts within the assembly.
Can you post a screenshot of your feature tree? I'm curious how you have this set up.Quote:
Originally Posted by FMJ
You're probably on the right track with this. Merging bodies in extrudes is a very useful tool until it isn't. Either way, I think a screenshot of his feature tree will explain a lot.Quote:
Originally Posted by StrawberryBoi
Ditto on the "Merge Result" selection box in the feature. Turn that off. You will still be able to do your booleans (add subtract intersection) operations but if you still want to keep the tool body go back and make a copy of the tool before the boolean operation.Quote:
Originally Posted by FMJ