I'm wondering if these features exist

RyanAvery

Is it possible to save selection of parts? I'm designing cabinets for my outfeed table and I want to select all the toekick boards, and group them into a selection. That way I can show / hide all the toekick boards easily. 

I know that I could just boolean combine them into 1 part and show / hide that, but I want them in individual parts so I know what lengths of boards to cut and how many, etc. 

Is it possible to quickly get a parts list of all parts in my studio? Basically I want something that shows me, for instance, the top / side / front view of each individual part and has 4x or 1x next to it to show me how many of that part I need to build. I know I can use the drawings feature but then I would have to do that for each part, but I want it to be done for me. Is there a plug in for this? 

Is there a way to see if any of my parts are overlapping? Currently, I move the camera around the parts and look for flickering colors to detect any overlapping. 

What is a good way to split a part into smaller pieces? Say you have a picture frame that is all one part, and you want to split it into the 4 parts that would make up a real picture frame, and they would be split at 45 degree angle at the corners. Currently to do this, I would make a sketch that overlaps the part and make all 4 45 degree angles in it, then I would extrude 4 parts from this in both directions for like 500 mm or something big just to make sure it overlaps. Then I would do four subsequent Boolean intersection operations to split my picture frame into 4 parts. 

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default? 

Is there a way to design custom hotkeys? For example making a hotkey to show / hide all sketches or "hide current selection" hotkey or a "hide all but selection" hotkey? 

3dcad

Is it possible to save selection of parts? I'm designing cabinets for my outfeed table and I want to select all the toekick boards, and group them into a selection. That way I can show / hide all the toekick boards easily. 

- You could use configurations but that's not really what they are there for.. I'm not sure if feature script could help you on this?
You could also create quick assembly of your toekick boards?

Is it possible to quickly get a parts list of all parts in my studio? Basically I want something that shows me, for instance, the top / side / front view of each individual part and has 4x or 1x next to it to show me how many of that part I need to build. I know I can use the drawings feature but then I would have to do that for each part, but I want it to be done for me. Is there a plug in for this? 

- Have you checked new Bom feature and OpenBom? I'd suggest to first create assembly  of your part studio and do all part duplicating there to get proper bill of materials. 

Is there a way to see if any of my parts are overlapping? Currently, I move the camera around the parts and look for flickering colors to detect any overlapping. 

- We don't have automatic collision detection feature at the moment, there should be an IR to vote though.

What is a good way to split a part into smaller pieces? Say you have a picture frame that is all one part, and you want to split it into the 4 parts that would make up a real picture frame, and they would be split at 45 degree angle at the corners. Currently to do this, I would make a sketch that overlaps the part and make all 4 45 degree angles in it, then I would extrude 4 parts from this in both directions for like 500 mm or something big just to make sure it overlaps. Then I would do four subsequent Boolean intersection operations to split my picture frame into 4 parts. 

- You can create surface or plane and use split feature https://cad.onshape.com/help/index.htm#cshid=splitpart

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default? 

- I don't think it's possible to change the defaults yet. This has been discussed at some point but I'm not sure if there's even IR for this.

Is there a way to design custom hotkeys? For example making a hotkey to show / hide all sketches or "hide current selection" hotkey or a "hide all but selection" hotkey? 

- Custom hotkeys are highly requested feature and Onshape knows it. Not available yet.

While waiting for new features, there's a LOT of workarounds and other wisdom shared in this forum. 

Jake_Rosenfeld

@RyanAvery

To answer your questions in order:

I do see the benefit of having some way to get a dialog to bring up previous parameters.  Maybe vote on Owen's request:
https://forum.onshape.com/discussion/8946/shift-enter-repeat-function-remember-previous-parameters
Or search around for another or post your own if you think it's different enough from what he wants.

If this is a very important workflow for you, you could make a copy of extrude.fs and extrudeCommon.fs and add the REMEMBER_PREVIOUS_VALUE ui hint to the definition.depth annotation, but I don't think this is the right approach because remember previous does not work for expressions that contain variables, and it seems like variables are key to your workflow.  Additionally, you would have to update your extrude document every time we push an update.

Another option for this that may serve your benefit would be to write a custom feature that takes a bunch of sketch selections and extrudes them individually based on their own sketch planes.  Then you could accomplish this thing in one feature rather than 20.  Remember that currently, if all your sketches are on different planes, but some of those planes have the same direction, you could group all the extrudes that go in the same direction.




Your second question could also be accomplished with a relatively simple FeatureScript feature.  You could iterate through all the parts in the Part Studio and take intersections of them (with "keep tools" on so that the original parts aren't deleted), then color all the created parts red or something.





Both of these features sound fairly interesting to write.  I'm not sure if I'll have time to get around to them, but I'll let you know if I do.  Otherwise, I could provide direction if you want to write them yourself.

3dcad

Is it possible to save selection of parts? I'm designing cabinets for my outfeed table and I want to select all the toekick boards, and group them into a selection. That way I can show / hide all the toekick boards easily. 

- You could use configurations but that's not really what they are there for.. I'm not sure if feature script could help you on this?
You could also create quick assembly of your toekick boards?

Is it possible to quickly get a parts list of all parts in my studio? Basically I want something that shows me, for instance, the top / side / front view of each individual part and has 4x or 1x next to it to show me how many of that part I need to build. I know I can use the drawings feature but then I would have to do that for each part, but I want it to be done for me. Is there a plug in for this? 

- Have you checked new Bom feature and OpenBom? I'd suggest to first create assembly  of your part studio and do all part duplicating there to get proper bill of materials. 

Is there a way to see if any of my parts are overlapping? Currently, I move the camera around the parts and look for flickering colors to detect any overlapping. 

- We don't have automatic collision detection feature at the moment, there should be an IR to vote though.

What is a good way to split a part into smaller pieces? Say you have a picture frame that is all one part, and you want to split it into the 4 parts that would make up a real picture frame, and they would be split at 45 degree angle at the corners. Currently to do this, I would make a sketch that overlaps the part and make all 4 45 degree angles in it, then I would extrude 4 parts from this in both directions for like 500 mm or something big just to make sure it overlaps. Then I would do four subsequent Boolean intersection operations to split my picture frame into 4 parts. 

- You can create surface or plane and use split feature https://cad.onshape.com/help/index.htm#cshid=splitpart

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default? 

- I don't think it's possible to change the defaults yet. This has been discussed at some point but I'm not sure if there's even IR for this.

Is there a way to design custom hotkeys? For example making a hotkey to show / hide all sketches or "hide current selection" hotkey or a "hide all but selection" hotkey? 

- Custom hotkeys are highly requested feature and Onshape knows it. Not available yet.

While waiting for new features, there's a LOT of workarounds and other wisdom shared in this forum. 

MBartlett21

3dcad said:

- I don't think it's possible to change the defaults yet. This has been discussed at some point but I'm not sure if there's even IR for this.

IR: https://forum.onshape.com/discussion/8946/shift-enter-repeat-function-remember-previous-parameters

owen_sparks

RyanAvery said:

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default?

I don't have anything to add to Rami's excellent reply but these 2 IR's may be of interest:-

https://forum.onshape.com/discussion/8946/shift-enter-repeat-function-remember-previous-parameters

https://forum.onshape.com/discussion/9050/copy-n-paste-features-in-the-feature-tree


Cheers,

Owen S.

Jake_Rosenfeld

@RyanAvery

To expand on a couple things said here already:

Is it possible to quickly get a parts list of all parts in my studio? Basically I want something that shows me, for instance, the top / side / front view of each individual part and has 4x or 1x next to it to show me how many of that part I need to build. I know I can use the drawings feature but then I would have to do that for each part, but I want it to be done for me. Is there a plug in for this? 

- Have you checked new Bom feature and OpenBom? I'd suggest to first create assembly  of your part studio and do all part duplicating there to get proper bill of materials. 

If you end up having parts that are exactly the same, it may end up being worth it to only build once instance in the Part Studio, and insert it multiple times in multiple places in your assembly.  This is what @3dcad means when he says to do all your part duplication in the assembly.  If you build multiple instances of things that match up perfectly in the Part Studio, and then insert them separately into an assembly, they will still show up as separate parts in either our built-in BOM or OpenBOM.

Is there a way to see if any of my parts are overlapping? Currently, I move the camera around the parts and look for flickering colors to detect any overlapping. 

If you are working in a Part Studio, you can do a Boolean Intersection between two parts that which you are concerned about overlaps.  If there is any material left over after the intersection, it is an overlap.
https://cad.onshape.com/help/Content/booleanparts.htm

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default? 

If you are doing a bunch of extrudes that match each other, you may be interested in the Variable feature:
https://cad.onshape.com/help/Content/variable.htm
This would allow you to set 20mm once, and then reference that number in all your extrude features.  If you then decide to change the 20 to a 30, you only have to change it in one place, and all the extrudes will follow.

You may also be interested in using Face or Feature option of Linear, Circular, and Curve pattern to make patterns of extrusions on a part.

3dcad

Jake_Rosenfeld said:

..  If you build multiple instances of things that match up perfectly in the Part Studio, and then insert them separately into an assembly, they will still show up as separate parts in either our built-in BOM or OpenBOM.

OpenBOM has feature to combine parts with same name - I'd still suggest to create assembly instances rather than part copies.

Jake_Rosenfeld

Thanks for clarifying Rami!

3dcad

RyanAvery

If you are doing a bunch of extrudes that match each other, you may be interested in the Variable feature:
https://cad.onshape.com/help/Content/variable.htm
This would allow you to set 20mm once, and then reference that number in all your extrude features.  If you then decide to change the 20 to a 30, you only have to change it in one place, and all the extrudes will follow.

You may also be interested in using Face or Feature option of Linear, Circular, and Curve pattern to make patterns of extrusions on a part.

Yes I agree, so say that I am about to do 20 different extrudes of the same distance (each extrude is on a different plane, however). So now I select the surface, shift + e to bring up extrude, then I have to click into the distance box, paste the name of the variable, then hit enter. Then I select a different surface, shift e, click distance box, paste name of variable. (because the default "1 inch" distance will show up in the distance box by default. What I was wondering if there was a way to make the default not be "1 inch" but instead "#varaibleThatWasUsedLast" because 100% of the time "1 inch" is not the extrude distance I will ever use, but 10% of the time "#varaibleThatWasLastUsed" is the correct distance, and I could just do shift + e and then hit enter. 

RyanAvery

If you are working in a Part Studio, you can do a Boolean Intersection between two parts that which you are concerned about overlaps.  If there is any material left over after the intersection, it is an overlap.
https://cad.onshape.com/help/Content/booleanparts.htm

Say I want to check any overlaps between 100 parts. I would have to do 100 different boolean operations to find all possible overlaps. If I just select all 100 parts and do boolean intersection, this would only leave me with places where all 100 parts overlapped at the same place (which is not likely to exist or help)

owen_sparks

Another less precise way is to go into section view and sweep down your model, anything intersecting will show up red.

Jake_Rosenfeld

@RyanAvery

To answer your questions in order:

I do see the benefit of having some way to get a dialog to bring up previous parameters.  Maybe vote on Owen's request:
https://forum.onshape.com/discussion/8946/shift-enter-repeat-function-remember-previous-parameters
Or search around for another or post your own if you think it's different enough from what he wants.

If this is a very important workflow for you, you could make a copy of extrude.fs and extrudeCommon.fs and add the REMEMBER_PREVIOUS_VALUE ui hint to the definition.depth annotation, but I don't think this is the right approach because remember previous does not work for expressions that contain variables, and it seems like variables are key to your workflow.  Additionally, you would have to update your extrude document every time we push an update.

Another option for this that may serve your benefit would be to write a custom feature that takes a bunch of sketch selections and extrudes them individually based on their own sketch planes.  Then you could accomplish this thing in one feature rather than 20.  Remember that currently, if all your sketches are on different planes, but some of those planes have the same direction, you could group all the extrudes that go in the same direction.




Your second question could also be accomplished with a relatively simple FeatureScript feature.  You could iterate through all the parts in the Part Studio and take intersections of them (with "keep tools" on so that the original parts aren't deleted), then color all the created parts red or something.





Both of these features sound fairly interesting to write.  I'm not sure if I'll have time to get around to them, but I'll let you know if I do.  Otherwise, I could provide direction if you want to write them yourself.

Jake_Rosenfeld

@RyanAvery

I actually just found this custom feature I wrote a while ago that executes all the selected extrudes separately:
https://cad.onshape.com/documents/cf2ebd36a36695408b9650a9/w/8e89a7bc10431e16fe2fceb7/e/859f48de91ab85a402b96e0c

I don't actively support it and it doesn't have any manipulators because of a weird selection bug, but maybe it'll be helpful for you.  It should do extrusions for every selection in reference to their own sketch plane.

To add it to your toolbar just press the "+" in the toolbar pane when you are visiting the document.

emagdalenaC2i

RyanAvery said:

Is there an option somewhere to make the default behavior of a dialog box default to whatever settings you chose the last time you used that dialog box? For instance, say I'm going to do 20 extrudes in different directions, but all of the same part and for the same distance. I do the first extrude, type in 20mm, then accept. Next time I open extrude, is it possible to have 20mm already in there as the default? 

Maybe you can try with Thicken instead of extrude ;-)

emagdalenaC2i

You will also improve your performance ;-)

Jake_Rosenfeld

@RyanAvery

Here is a custom feature I threw together for detecting part overlaps:
https://cad.onshape.com/documents/4ef9d7bf5c04de6c159e6fb0/w/50103cbdb65f20d04d6f68f1/e/e4e11c6e5f2327384ab0fe86

YMMV; it'll probably get pretty slow for part studios with many parts (Its time complexity is O(number of parts^2)).

emagdalenaC2i

Nice. Great tool!! 

MBartlett21

Jake_Rosenfeld said:

@RyanAvery

Here is a custom feature I threw together for detecting part overlaps:
https://cad.onshape.com/documents/4ef9d7bf5c04de6c159e6fb0/w/50103cbdb65f20d04d6f68f1/e/e4e11c6e5f2327384ab0fe86

YMMV; it'll probably get pretty slow for part studios with many parts (Its time complexity is O(number of parts^2)).

@Jake_Rosenfeld
@Ryan_Avery

I have extended that custom feature and you can now trim the parts to not intersect
https://cad.onshape.com/documents/be4d0a14bee7c3ec752a6fea/

emagdalenaC2i

@mbartlett21 great improvement

Jake_Rosenfeld

Thanks @mbartlett21!

I avoided doing that because the only way I envisioned it was to cut from both the parts.  Nice solution with the extra selection box!

Jake_Rosenfeld

@mbartlett21

I'm wondering what the desired behavior here is when two intersecting parts are both selected into "Trim parts".  As of now, your code creates a void by subtracting the intersection from both the parts.  Is this desired, or would the user rather the system have some way of picking only one to subtract from?