After you copy a part edit becomes poor

don_b

Where as this is a fantastic product in many ways it is missing some basic features ......if one is to modify part 1 of the sample ...part 2 changes....you can not edit part 1 only....to edit part 2 requires that you essentially rebuild part 2 from scratch....See my idea about a part owns the sketch and it is copied with the part for easy edit.
https://cad.onshape.com/documents/67b621172175ec77ca607f33/w/303859a18fe9fd7318879c5d/e/2b146c98035a6f38338ef6a5

don_b

https://forum.onshape.com/discussion/20682/sketch-new-sketch-attached-to-part-for-easy-edit-after-translate-copy#latest

_anton

This really depends on what you're trying to do.

If you're trying to make a family of parts, you probably want to use configurations instead. If you need to replicate a few simple sketches, you could feature-pattern them, using their entities as reference for whatever changes you want to make. And, if you're just translating a part, it tends to be more correct (in the paradigm of parametric CAD) to just move the creating sketch instead.

If you need something more complicated, you could write a custom feature that replicates sketches as well.

bryan_lagrange

@don_b here is a simple configurations family of plates. It is one model plate that can be configured to different sizes and holes sizes. I also put a drawing to show that one modeled part can produce multiple drawings of different plates with different configurations.

Are you looking to do something similar to this?

https://cad.onshape.com/documents/6390586dec6602eece0da9c8/w/63b6b958b64289c96fdc102a/e/02739df532dca6de08b46417

don_b

Thank you for your interest...ok learned something ....I just want to copy and then be able to edit....and perhaps the secrete is to make simple parts and add/subtract  features afterwards.....as long as I do not alter the original sketch it is possible to then edit the original part  using extrude remove or boolean and on the copied parts too..of course if the original part has holes one might have to perhaps fiddle with the rollback bar which I have not tried yet but seems very complicated as    "all I want to do is copy a part and be able to edit the original part and the new part easily".
This program is very extensive but that seems to be something any CAD program should be able to do without resorting to special programming on the part of the user or convoluted order of operation to     "just edit a part"

bryan_lagrange

You can do a lot with configurations. Here is a "dirty little samples" that I used to fail features to configure different parts.

https://cad.onshape.com/documents/75212da89ad605aa969ac55e/w/f6490e913c9be236b92c0151/e/057e2528798ef9bee4715b3c

eric_pesty

don_b said:

Thank you for your interest...ok learned something ....I just want to copy and then be able to edit....and perhaps the secrete is to make simple parts and add/subtract  features afterwards.....as long as I do not alter the original sketch it is possible to then edit the original part  using extrude remove or boolean and on the copied parts too..of course if the original part has holes one might have to perhaps fiddle with the rollback bar which I have not tried yet but seems very complicated as    "all I want to do is copy a part and be able to edit the original part and the new part easily".
This program is very extensive but that seems to be something any CAD program should be able to do without resorting to special programming on the part of the user or convoluted order of operation to     "just edit a part"

If you just need to copy a part and make changes the "normal" process would be to duplicate the part studio. If you want to make small changes to a copied part, there are a number of "direct editing" tools that can do that without needing the original sketches (mainly delete/move face).

I believe you are doing a lot of work "all in one part studio" but that might not be the best option based on what you are trying to achieve...
I have a felling you might be better served by using other "top down" design approaches like deriving in reference geometry (sketches, faces, or even bodies) or using assembly contexts.

As a general rule if you find yourself needing functionality that no one else is asking for, it might be a sign you are not using the tool in it's "intended way" and there might be better approaches...

Also if the rollback bar is "very complicated", you might want to take a look at this: https://learn.onshape.com/learn/course/introduction-to-parametric-feature-based-cad/what-is-cad/parametric-feature-based-cad?page=1

don_b

thank you and I admit to serious ignorance ....I will try to be better in the future....I have used move face, but not delete face...I will have to play with that...I have used derived parts but not sure about what you mean "in reference geometry." unless it is "putting it where it needs to go" which I have been able to do. I have not used configurations and instead just copy and change the name in case what I am playing with needs to go back to a previous version....I looked at the above configuration sample and am at a loss as to why all those different configurations could or would not be tried out in the part studio to arrive at a desired geometry. Just draw it and translate it and draw another and delete what you do not want without using configurations but I must be missing something...and I exaggerate about the roll bar I have altered placement of  features with the rollbar to get desired results. ....I miss simple cad....no separation of features between say the sketch routine and part studio and assembly studio. .....one screen with all the features usable....or at least a unified part studio ...I can see that movement in the assembly studio could be too confusing in the part studio as it certainly could screw up reference geometry.    I have taken this on because my new wing has much geometry in compound angle geometry and calculating flat patterns  looks like it might be a thing of the past for me because of this program.....Thank you again for your help.

eric_pesty

I think one of the key issues that "philosophically" the whole concept of "copy-move-edit" doesn't really fit in the context of parametric design. That's the way things work in Autocad but it's jut not very efficient.

I've tried to come up with a better example of ways to use configurations, variables and "reference". It's a bit rough because I didn't spend much time on it but hopefully it gives you some usable ideas...

https://cad.onshape.com/documents/63ede05284ce595591bb58b9/w/c90c3f825e72564dfccfaf0c/e/316778b4dc2bd074d20d0bd1?renderMode=0&uiState=6438a33afe0fad7411cef349

If you look at this assembly, there are three instances of the "configured bracket". These parts are configuration of the same part so use the exact same features, which is a much better way of doing things than copying and modifying when you have variations of the same geometry. In this case I used configuration variables so that these are "infinitely adjustable". I could also have opted for a table generating a set number of parts of specific dimensions.

In this case I created a "reference" surface which was created as an in-context part from the assembly, which is itself controlled by the two layout sketches I imported (one for the root and one for the tip). To make things interesting I made it as a loft so the taper isn't constant.

I am using the "reference shape and measurement ref" part studio (which is where I initially created reference surface) to "read" the values to use for each bracket (based on the distance from the root, which is also set with a variable), I can then go and "edit configuration" of each bracket in the assembly and set the values based on the measured ones. This method is actually not "parametric" as I have to set these manually but that can sometimes be useful if you want more detailed control (see example gif below).

As another example I also created a quick and dirty example part using the same reference geometry derived into the "Moved reference example" part studio. In this case I use a transform to move the reference geometry (using a configuration variable again) and create the brace part (rather than move the part, move the reference so the origin of the part remains constant). When I insert the brace part in the assembly, I just have to mate it to the reference surface corner (using the mate connector I created in the part) and it will always be the correct size and at the correct location based on the configuration it is set to.
This is "true" parametric design where I can put a brace anywhere from drawing the part just once and I adjust one value to create a new one in a different spot. It's a little bit more work up front for a lot less effort down the road...

dirk_van_der_vaart

@don_b
I think you are looking for the Derived feature
https://cad.onshape.com/help/Content/derived.htm?Highlight=Derived
https://learn.onshape.com/courses/master-model

don_b

eric_pesty said:

I think one of the key issues that "philosophically" the whole concept of "copy-move-edit" doesn't really fit in the context of parametric design. That's the way things work in Autocad but it's jut not very efficient.

 Well I certainly am learning that....and you have really done some work here for me (complete constructions gifs... very impressive)....What you are doing I would imagine would be considered advanced techniques ....but maybe not.... the list would have to comment on that.....Possible Improvements  for me would be to use configurations at different wing locations to build my similar parts.....try to learn variables to change the similar parts......and try to make use of the assembly tab rather than everything in one part studio tab.

I would need  flat patterns and more massage of the part will be required although my thread on transform and edit sheet metal parts does have workarounds for that..... no criticism intended.  

Your example shows a whole different work flow and philosophy ......its hard for old dogs to learn new tricks....    

Thank you very much.

don_b

dirk_van_der_vaart said:

@don_b
I think you are looking for the Derived feature
https://cad.onshape.com/help/Content/derived.htm?Highlight=Derived
https://learn.onshape.com/courses/master-model

I have used Derived parts ....inserted a rivet into a part studio for example..... 

don_b

bryan_lagrange said:

You can do a lot with configurations. Here is a "dirty little samples" that I used to fail features to configure different parts.

https://cad.onshape.com/documents/75212da89ad605aa969ac55e/w/f6490e913c9be236b92c0151/e/057e2528798ef9bee4715b3c

how did you get the versions out of "versions are view only"?

bryan_lagrange

If you make a copy of the Onshape document you should be able to have write access.

glen_dewsbury

@don_b
To retrieve a version to main. Select main in the version list. Right click on the version you want to retrieve and a menu will display. Select restore to main.

don_b

If you want to see why I think this is so poor as regards edit .....just try to remove the holes and have it reflected in the flat pattern or even make a drawing of the flat pattern where the flat pattern sits square to the paper.....

https://cad.onshape.com/documents/9e2e1b002f638eda4ef66d49/w/982beac394793812088a1db3/e/380910d584491a9e114e6a47

It probably is possible but I will  do it when I export to my Autocad the flat pattern....very frustrating here

and those sheet metal parts were all designed in the part studio and if you could do them in individual part studios you are a better designer than I am

don_b

The part needs to own the sketch or a copy of the sketch  for easy edit

eric_pesty

@don_b
There is so much wrong with the entire model that I don't know where to start... A number of us have been trying to help by providing pointers on how to do this "properly" but if you insist on creating 100s of part with over a 1000 feature in a single part studio (including a bunch of redundant, broken ones), you are going to have a bad time!

Assuming we are talking about "sheet metal model 29" if you don't want some of the holes just create the part from sketch 428 (instead of the face of the solid) and select whichever faces you need, very simple...
And if you want to export a DXF with a specific alignment, just put that part into a drawing and use "align" view to pick a horizontal edge and export that. Also very simple.

If you are just doing a simple part you can get away with "freestyling" but not something like this. You are trying to design a complex assembly without first taking the time to understand the basic concepts of parametric CAD or following any of the best practice so it's no wonder it's not going smoothly!

If you would just go through the "top down" learning pathway in the learning center (and whatever other courses you need to get to the level where you can actually understand it), you could learn a number of different ways you could break this down into manageable chunks and design parts (or groups of parts) in separate part studios.

Basically this is like watching someone try to chop down a tree while holding the axe from the wrong end! Feel free to continue attempting doing this "your way" but please don't blame the tool if you are not willing to learn how to use it first!

don_b

I do apologize my ignorance and anger is also poor...I appreciate your attempts to help and the time you must have spent. 

don_b

I am almost ready to export the drawings to Autocad 14 where my 24x36" plotter resides in a virtual XP (no drivers later versions)  I only need to plot accurate flat patterns of parts in compound geometry which is a real pain in 2D and prone to errors .....I am reminded of the movie "Grumpy Old Men" 
I certainly will be able to massage the drawings in the Autocad in about 2 minutes 
Sorry but the time invested in this drawing I feel I can save time by struggling rather than starting over ...
I would hope my struggles and comments might have  helped the development of this platform as I still am very impressed ....