Solidworks
September 09, 2012 11:26AM
I want to create a two part item to be printed but when I use the finished part 1 to make sure the parts in part 2 line up they become one part which I don't want. How do you make a multi-part assembly knowing the parts line up in Solidworks?
Re: Solidworks
September 09, 2012 12:09PM
At a guess, since I'm afraid I don't know solidworks too well, make then into a block structure. AFAIK, even in solidworks, blocks should retain their own individuality. I'm not exactly SURE that's how it works in solidworks, but hopefully this will get you looking in the right direction.

If not, sorry for the spam winking smiley
Re: Solidworks
September 09, 2012 01:23PM
If I understand what you want, make two versions of the part, different names.

first put a cut plane or feature on the seam of your division.
then, save as a second name
on one part, cut off in one direction
in the other, cut off in the opposite direction

make an assembly and put them both on the Csys.

kind of a brute force way to do it.

Usually, I just avoid the assembly check and cut one way, save as an STL, then reverse the cut, save as another STL.
I don't any air gap in the cuts. I used to use .005in of air, but quit.

hope that was on track.

Dave
Re: Solidworks
September 09, 2012 02:25PM
What you want is a multibody part.

When you extrude a part there is a little check box that says "merge"

If you un-check it, that extrusion becomes it's own separate body.

Look up multibody part tutorials and it should become fairly obvious how it works. You can even copy, add, subtract and combine those bodies to do some really cool stuff that would otherwise be very complicated.

When you are ready to export your file, simply delete the body for material A and export, then go back and delete the body for material B instead, and export. The coordinate systems should remain identical.


www.Fablicator.com
Re: Solidworks
September 09, 2012 04:05PM
Nope, the merge result has nothing to do with this issue.

See, if I create a hole in the body then make a separate plane and create a extrusion that is directly over the hole that extrusion is linked to the main body even though I don't want it to be. I know it is linked because I suppress the main body and POW the extrusions get suppressed as well.

All I want is to use the main body as a reference when creating the second body but lay anything down that is directly over the other body and it suddenly becomes linked which is not what I need.

Any ideas?
Re: Solidworks
September 09, 2012 05:06PM
the merge check makes multi body parts well.
When you add new features, you merge them to a specific body or all bodies.

the attached image shows a two body part, one is pink and the other is green. this is one part, not an assembly.
a new wall extrusion feature is merge checked, and I am only joining it to the one body not the other. After done, i still have a two body part, but the wall is now attached on one body. The other is just there.

i still am not sure your question to be honest.

designing multiple separate parts in assembly is the preference. Don't create parent/child relations if you are worried about linking.
relations that are external have a --> indicator next to them in display relations, or filter just external and delete, or hold control button to not have relations snap to anything.

maybe you could attach a sample file.

I'm sure we could sort out your question, over a pint or two.

Davesmileys with beer
Attachments:
open | download - idea.jpg (102 KB)
Re: Solidworks
September 09, 2012 06:20PM
Suppressing will also suppress anything based off of it, so it's no surprise that everything disappears. You need to hide the body that you don't want, rather than suppress it. I do this quite often, where I start with another part, extrude off of it but don't merge it, then hide the original part. It works well. Anything that is hidden will not get exported when you save to STL.


Cameron

Help improve the RepRap wiki!
Just click "Edit" in the top-right corner of the page and start typing.
Anyone can edit the wiki!
Re: Solidworks
September 09, 2012 06:22PM
What I have is an revolved sphere with the bottom extrude cut flat. Now on that bottom I have 3 holes 5mm deep. Done part 1. Now I want to make a part that the holes line up and I extrude a 5mm circle up ( think slot A tab B ). When I make the circles no issues but as soon as I line them up with the holes it becomes a child. It doesn't show it is a child but when I go to suppress the sphere the new part should not go with it and by doing so it tells me they are linked. I even shoved the entire first part (the flat on one side sphere) into a folder and the new part is not in a folder but the same thing. Maybe using the same plane (top) to derive the second part's plane is causing a link?

edited: Stupid smileys.

Edited 1 time(s). Last edit at 09/09/2012 06:23PM by Dark Alchemist.
Re: Solidworks
September 09, 2012 06:42PM
yes, you have parent/child issues.

make sure what you click on is from the second part.

Also, if you see the -> there is an external link.
Attachments:
open | download - idea2.jpg (44.4 KB)
Re: Solidworks
September 09, 2012 07:22PM
Well, what can I do about it? As I said I have a completed part so I make a new plane offset 50mm from the top plane (this gets me to the bottom flat surface) and I use the new plane to make my new part. There is no external links since everything has been done in one session but I can't stop it from making the new part a child (in the tree it doesn't show it is a child but suppress the sphere and the new part will go suppressed as well) if I lay anything exactly over the bottom of the sphere.

I never had these issues in any of the 3d art programs so I hope it is easy to avoid in SW.
Re: Solidworks
September 09, 2012 08:03PM
Dark Alchemist Wrote:
-------------------------------------------------------
> I never had these issues in any of the 3d art
> programs so I hope it is easy to avoid in SW.

By creating a plane based off the completed part, then using that plane for your new part, you are creating a link. The plane cannot exist without the completed part, and therefor your new part cannot either. You can just hide the completed part though instead of suppressing it for the same effect without suppressing everything in the chain.


Cameron

Help improve the RepRap wiki!
Just click "Edit" in the top-right corner of the page and start typing.
Anyone can edit the wiki!
Re: Solidworks
September 09, 2012 08:10PM
I thought that might be the case because it is logical but isn't there a way to break that link? I mean I will have to at some point as I need two separate parts in two individual files soon.
Re: Solidworks
September 10, 2012 12:38AM
You can't break the link because the plane is defined by the previous part. If you remove the previous part, you lose the definition for the plane. To get individual parts, just save the whole thing twice. Hide the original part in one of them, and hide the new part in the other. You effectively then have two different parts, and they will behave that way too.


Cameron

Help improve the RepRap wiki!
Just click "Edit" in the top-right corner of the page and start typing.
Anyone can edit the wiki!
Re: Solidworks
September 10, 2012 12:41AM
When I hide them will they both show up in the tree when I load them separately?
Re: Solidworks
September 10, 2012 02:04AM
Yes, they will still show in the tree, but greyed out. They will behave as if the greyed out part does not exist. It is necessary to do this if you want to have one part based directly off of another. If you remove the part or suppress it instead of hiding it, you have removed the basis for the new part, which will cause a rebuild to fail.

Art type modelling programs work quite differently, as you have found out.


Cameron

Help improve the RepRap wiki!
Just click "Edit" in the top-right corner of the page and start typing.
Anyone can edit the wiki!
Re: Solidworks
September 10, 2012 06:56PM
Just finished my construction and the hide/show worked beautifully when saving.

Thank you to everyone who offered their advice. smiling smiley
Re: Solidworks
September 10, 2012 11:18PM
Not a problem. I've been using SolidWorks for years, although there is still tons I do not know. I would not even know where to start with something like Blender or other other mesh modelling software.


Cameron

Help improve the RepRap wiki!
Just click "Edit" in the top-right corner of the page and start typing.
Anyone can edit the wiki!
Re: Solidworks
September 14, 2012 02:11PM
I would not recommend using hide in this way in general practice. You can get very offensive unintended picks and details when you import models with hidden features into a drawing later and the drawing view usually automatically expands to include the hidden objects too. It is also less efficient memory-wise which probably doesn't matter here, but it can make a big difference in large assemblies.

Anyway - "Delete body" also works and maintains the previous references by "deleting" the body with a feature lower in the feature tree. You can find "Delete body" under Insert->Features->Delete body...

You could also break the references once your features are lined up by using a plane offset from one of the original primary planes (instead of the part) and then delete the "on edge" or "coincident" linked references in the sketch using "Display/Delete relations" while in the sketch. Then you can remove all of the extraneous previous features and save separate parts, but your hole/feature locations will be totally independent betweent the two parts going forward.
Re: Solidworks
September 14, 2012 03:51PM
Would you explain a bit more on your second method because I always start on one of the original reference planes and anything I attach to that plane becomes attached to everything.
Sorry, only registered users may post in this forum.

Click here to login