How to deal with un-fixed parts in Assembly's

brucebartlett

My go to workflow for the start of an assembly is a Group Mate and Fix 1 part to lock things down but these are not always applicable when woking out the desired mechanism.

Sometimes parts that have come into the assembly in position from the part studio get moved and I don't find it easy to get them back to position. I also find myself moving parts to see what's constrained and whats not, then using undo to return parts to position, you are in trouble with this if the undo is missed.

How do others deal with unfixed parts in an assemblies when accidentally moved out of position?

3dcad

@brucebartlett Of course it depends on how big project you have but I have found myself simply deleting the unintensionally moved part and insert again.

Narayan_K

Hi@ brucebartlett , You can also get the original position by restoring the history.

3dcad

@Narayan_K The problem with history is that you lose work that is done after accidentally moved a piece. I remember having conversation about selectable history restoring regarding to something else with Onshape, that would serve this purpose too. 

@viru When you say 'fix constrain' do you mean actually fix or group mate? If you use fix to constrain things together you will have problems if that assembly is used as subassembly since fix doesn't apply in parent assemblies.

Best way to keep stuff together is to use group mate but it tends to forgot sometimes if you begin assembly with incomplete part studio and keep adding parts one by one and check assembly in between. 

+1 for 'Restore selected part(s) in Part Studio position'

gonzalo_chomon

I think the best for you is to take a look to one of the training videos that explains the basics of Asemblies here: https://www.onshape.com/learn/essential-training-series#!lesson-number=4&title=assembly-basics
And join this class: https://www.onshape.com/assemble-onshape-oct-1

shanshan

brucebartlett ,kindly remind you
 1) when you can not get the part back to position, you can suppress it ,and check if some mate feature turn red,so you will know if it is constrained or not.
2) in the mate feature window ,we just can "offset" the first mate connector,but if we create a mate connector first, in the mate connector window , we can "move" the mate connector,it includes "offset "and "rotate about any Axis",so you can adjust more data

 

3dcad

@brucebartlett Of course it depends on how big project you have but I have found myself simply deleting the unintensionally moved part and insert again.

brucebartlett

Hi thanks for the answers.

In this case I  deleted the part and re inserted again as @3dcad mentioned. There were however mates connected to this part which had to be re done, that was what I was trying to avoid. I did briefly look for a reset part to origin, this may be a nice feature to have. 

viru

@brucebartlett ,Inserting all parts in assembly I always give fix constrain to them. After that I make unfix to one part and give them constraint as per their functional requirement. Similar thing I am doing for all remaining parts one by one. Therefore there will be no chance for parts moved out of position in an assemblies. With the help of part suppress or hide also you can see what's constrained and whats not given to respective part and position also. I hope this will be helpful to you.

Narayan_K

Hi@ brucebartlett , You can also get the original position by restoring the history.

3dcad

@Narayan_K The problem with history is that you lose work that is done after accidentally moved a piece. I remember having conversation about selectable history restoring regarding to something else with Onshape, that would serve this purpose too. 

@viru When you say 'fix constrain' do you mean actually fix or group mate? If you use fix to constrain things together you will have problems if that assembly is used as subassembly since fix doesn't apply in parent assemblies.

Best way to keep stuff together is to use group mate but it tends to forgot sometimes if you begin assembly with incomplete part studio and keep adding parts one by one and check assembly in between. 

+1 for 'Restore selected part(s) in Part Studio position'

brucebartlett

The other way around this is to place a mate reference at the origin in the part studio, linked to the desired part. Then you can do a fasten mate to the origin in the assembly.  

andrew_troup

Nice useful tip, thanks @brucebartlett

It would indeed be good to have a  'Restore selected part(s) to Part Studio position'

shashank_aarya

+1 for 'Restore selected part(s) to Part Studio position' For this it is also required to identify which of the parts are not having any constrains. Currently to identify such parts we have one workaround of suppressing the individual parts in assembly to see if any related constrain is failed. But this can be time consuming when there are larger number of parts or sub assemblies in assembly structure. So, it would nice to have some icons to the parts which are also constrained, so that user can select those parts without any icon (unfixed parts) and restore them to part studio position as mentioned by @3dcad and @andrew_troup

viru

@brucebartlett , +1 for "reset part to original position" feature.
Previously similar option is available in assembly as shown in below link.
https://forum.onshape.com/discussion/306/improvements-to-onshape-january-27th-2015
(In addition to the origin in Assemblies, you can now use the manipulator to move selections to the origin, rotate 90/180 degrees about any axis or align/anti-align to Z on any manipulator direction).

@3dcad ,I am using "fix" option only at initial stage after inserting of part in assembly after-that "unfix" part one by one and giving constraint as per their functional requirement. At the end non of the parts in assembly is containing "fix" option and all the parts in assembly should contain at least one mate constrain as their functional requirement. By using this method user can know how much parts remained to give constrain in assembly which is equal to parts having "fix" symbol. It also avoid unnecessary movement for parts at the time of assembly creation .
Kindly refer below video for more clarification.

andrew_troup

That seems to me a smart workflow for the current state of the Onshape app, @viru.
Thanks for sharing it.

3dcad

@viru ok now I understand your workflow with fix.