Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Functionality needed for metal casting (and plastic part design)

pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
edited February 2015 in Product Feedback
I've submitted tickets for the following functionality and I'm sure others have for some or most of it as well.  I've been re-modelling a design in Onshape for a decently complicated metal casted component that I recently just finished in SolidWorks.  I wanted to see where all the pain points are.  I can't go too far at the moment because of lacking capability (split line and Parting line Draft).  Here is what I need in order to be happy with metal casting design (and plastic molded part design as well):  I have ranked them in order of most urgent in my eyes...

-  Split Line or Split Face tool:  This is needed to create parting lines to control the drafted faces.  In my workflow I generally put this just above the draft features, and before the fillets - but not always.  It would be nice to split with a sketch, surfaces, planes, and the intersecting edges of bodies.  Sketches would be priority and the rest as time allows.

-  Draft  - Parting Line Method (with stepped draft for those nasty bits...):  The parting line draft tool almost goes hand in hand with the split line/face tool.  If I can't have a parting line draft tool, then split line is almost useless at this point.

-  Base part: - I really like using the base part method.  I detail up a casting in a separate, clean, isolated file (I know, I know, files really go away in Onshape but its a habit).  I then insert that part into a blank file and complete modelling the machining features.  This keeps the data management nice and clean.

-  Draft Analysis:  Parts can get really complicated and its easy to forget adding draft to a face.  Casting vendors use this tool like crazy, too...

-  Thickness Analysis:  Ditto above.

- Geometry Compare:  I really like comparing a casting design to a machined casting design using a geometry compare.  I can quickly check to make sure all my machining allowances are proper - not too much, not too little.  I also use this for getting an amount of material removed, which is really useful for costing estimations based on material removal rates ($/lb of removal).


«1

Comments

  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,099 PRO

    -  Base part: - I really like using the base part method.  I detail up a casting in a separate, clean, isolated file (I know, I know, files really go away in Onshape but its a habit).  I then insert that part into a blank file and complete modelling the machining features.  This keeps the data management nice and clean.


    @Pete Yodis What would the disadvantage of doing this in the 1 part studio?  eg. built the cast part, copy and add the machining detail and custom properties (need more that the current list) to the new part.

    All other feature are need, I am sure they will come in time. I don't do very much of this work but have defiantly looked for the split line and draft tools.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    edited February 2015

    -  Base part: - I really like using the base part method.  I detail up a casting in a separate, clean, isolated file (I know, I know, files really go away in Onshape but its a habit).  I then insert that part into a blank file and complete modelling the machining features.  This keeps the data management nice and clean.


    @Pete Yodis What would the disadvantage of doing this in the 1 part studio?  eg. built the cast part, copy and add the machining detail and custom properties (need more that the current list) to the new part.

    All other feature are need, I am sure they will come in time. I don't do very much of this work but have defiantly looked for the split line and draft tools.
    @BruceBarlett The problem is when changes occur to the casting, I need them to ripple to the machining.  If they are not in two separate "files", how is that accomplished?  I would have to make a change to casting only model and then again to the casting and machining model.  I need the changes to propagate, like a part would change in an assembly file.

    The other features will no doubt come in time.  Thought I would share where I am at.
  • Ben_Ben_ OS Professional, Mentor, Developers Posts: 286 PRO
    edited February 2015
    Some things are already there:
    1. Split part: https://cad.onshape.com/help/#splitpart.htm
    2. Draft https://cad.onshape.com/help/#draft.htm
    3. Base parts: granted this is not parametric but try duplicate tab: https://cad.onshape.com/help/#introduction.htm or play with the branching and merging so see if there is a workflow in that. https://cad.onshape.com/help/#versionmanager.htm
    Food for thought...

  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,099 PRO
    Good one @Ben, I forgot about the draft command. 

    @BruceBarlett The problem is when changes occur to the casting, I need them to ripple to the machining.  If they are not in two separate "files", how is that accomplished?  I would have to make a change to casting only model and then again to the casting and machining model.  I need the changes to propagate, like a part would change in an assembly file.
    Pete, I would do this by rolling back to just above the copy on the tree in the part studio, that way any changes blow through to the machined casting. I don't see why this would not work as well as method you use in Solidworks. I will try and do an example.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • kevin_quigleykevin_quigley Member Posts: 306 ✭✭✭
    edited February 2015
    Ben draft in Onshape right now is basic from face only. Not from parting line. Makes doing a lot of detail part design work impossible. Yes you can draft if you have a flat surface or plane but not from a curved or stepped split line.

    to be a useful part design tool for production use in injection moulding or casting you need split line capability. Split line tool is also essential for many other tasks relating to surfacing.
  • caradoncaradon OS Professional, Mentor Posts: 300 PRO
    Yep. Split line is essential.
    I find myself missing it every day I use Onshape.

    Dries
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,585 PRO
    I would like to add this one to Pete's list.

    -Extrude Draft: All add, new, remove, surface need to have this option.


  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 631
    This is rather interesting timing as one of our members here gave a presentation last Wednesday about molds and frustrations that mold engineers have with traditional CAD systems.  It gave us a lot to think about.

    As usual, specific workflows or examples are useful in determining what and how it should be implemented.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • kevin_quigleykevin_quigley Member Posts: 306 ✭✭✭
    Jake, that statement is a worry to me. this functionality is needed for basic design, not just for doing moulds. Split line is used for many many modelling tasks aside from creating mould split lines.

    OnShape is not a serious modelling tool unless it has this functionality. I for one expected Onshape to be pushing the boundaries of what creating geometry means. Currently this is not happening. You are pushing boundaries on the delivery mechanism of the system to the user. But that is pointless if the tools they have available are unable to create what they want. You need both.
  • Ben_Ben_ OS Professional, Mentor, Developers Posts: 286 PRO
    edited February 2015
    I agree @KevinQuigley however sometimes we need to take a step back and have a look at the current toolset and see if there is a way to do what we need outside of the paradigm that is ingrained in our minds. The single biggest thing I have taught to people using SolidWorks is to ignore the name of the function you are using and look at what it does. The best example is when in SW to use the mold cavity tool in assembly weldments to make cuts. The tool was not designed to work in weldments but it was critical to my workflows in weldments. 

    So back to my point. How do we take these rudimentary tools we have and create a workflow to do what you need. Even if it is long and arduous. The reason is it will give the developers a workflow to base the next iteration of changes on this sort of workflow. I fully get that it is a PITA but in the end the benefits of letting these guys into our minds is a awesome tool in the end we all love.

    We have taken the first step by identifying tools that sort of do what we need and suggested the improvements to get them to the next step. For example:

    "Onshape right now is basic from face only. Not from parting line. Makes doing a lot of detail part design work impossible. Yes you can draft if you have a flat surface or plane but not from a curved or stepped split line. to be a useful part design tool"

    I think the next step here is to let them see about doing curvy split lines and draft combinations. Given how fast and furious changes have been coming I bet it will be implemented in short order.

  • lougallolougallo Member, Moderator, Onshape Employees, Developers Posts: 1,938
    @KevinQuigley Not to worry.. There are a number of workflows for many of the aforementioned tool sets.  Split line tools I have used for complex parting lines, face breaks for applying simulation boundary conditions as well as ways to break surfaces for reliefs, logos and other thicken/embossing processes.  The topic here was molds and having specific workflows allows these tools to be designed with these workflows in mind to ensure the feature addresses these needs.  
    Lou Gallo / PD/UX - Support - Community / Onshape, Inc.
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    Good one @Ben, I forgot about the draft command. 

    @BruceBarlett The problem is when changes occur to the casting, I need them to ripple to the machining.  If they are not in two separate "files", how is that accomplished?  I would have to make a change to casting only model and then again to the casting and machining model.  I need the changes to propagate, like a part would change in an assembly file.
    Pete, I would do this by rolling back to just above the copy on the tree in the part studio, that way any changes blow through to the machined casting. I don't see why this would not work as well as method you use in Solidworks. I will try and do an example.

    @BruceBartlett I'll take a look at that method.  Thanks.
  • douglas_1douglas_1 Member Posts: 7
    I agree with this thread wholeheartedly.  I use the base part workflow for adding secondary machining to injected molded parts.  A better draft feature, better splines and complete SURFACING**** is needed for me to complete just about any typical project. 
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    @BruceBartlett I'm not seeing the copy part command in my feature toolbar.  Do you see it?  The help at the moment shows it in the feature toolbar, but its not there.  I can still copy part from the tree.  Looks like this method will work.  I do have to make sure I select the proper body to cut for each cut feature on the machining of the casting.  Slightly kludge, but I think it will work.  It's not entirely clear from the tree what is going on with the parts, so I would worry that those invited in to review the design might not get what is constructed quickly and easily.  That it is the nice thing with derived or base parts.  Very clean.  Very obvious to all involved.  The copy part method seems a little too stealthy in my opinion.
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 631
    @BruceBartlett I'm not seeing the copy part command in my feature toolbar.  Do you see it?  The help at the moment shows it in the feature toolbar, but its not there.  I can still copy part from the tree.  Looks like this method will work.  I do have to make sure I select the proper body to cut for each cut feature on the machining of the casting.  Slightly kludge, but I think it will work.  It's not entirely clear from the tree what is going on with the parts, so I would worry that those invited in to review the design might not get what is constructed quickly and easily.  That it is the nice thing with derived or base parts.  Very clean.  Very obvious to all involved.  The copy part method seems a little too stealthy in my opinion.
    Copy part has been replaced with Transform's option "Copy in place".
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,099 PRO
    @BruceBartlett   Looks like this method will work.  I do have to make sure I select the proper body to cut for each cut feature on the machining of the casting.  Slightly kludge, but I think it will work.  It's not entirely clear from the tree what is going on with the parts, so I would worry that those invited in to review the design might not get what is constructed quickly and easily.  That it is the nice thing with derived or base parts.  Very clean.  Very obvious to all involved.  The copy part method seems a little too stealthy in my opinion.
    @Pete Yodis Onshape has been designed around part studio to be able to link parts together, once a user is clear on how to use Onshape part studio's I think this method should be clear. I also hope over time Onshape will improve the feature tree and parts list. I had this idea about clicking on a part and highlight features in the feature tree, see https://forum.onshape.com/discussion/comment/1565/#Comment_1565

    Another method I've seen work in Solidworks is to drop the the casting into an assembly and add the machining processes with cut extrudes and hole feature's. I'd like to think Onshape will have this functionality in their assemblies also in the future and could be a work around if added however I think their need's to be the ability to add parts in a part studio, I have often had the need to add an imported part into a part studio.  
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    @BruceBartlett I'm not seeing the copy part command in my feature toolbar.  Do you see it?  The help at the moment shows it in the feature toolbar, but its not there.  I can still copy part from the tree.  Looks like this method will work.  I do have to make sure I select the proper body to cut for each cut feature on the machining of the casting.  Slightly kludge, but I think it will work.  It's not entirely clear from the tree what is going on with the parts, so I would worry that those invited in to review the design might not get what is constructed quickly and easily.  That it is the nice thing with derived or base parts.  Very clean.  Very obvious to all involved.  The copy part method seems a little too stealthy in my opinion.
    Copy part has been replaced with Transform's option "Copy in place".

    Got it.  Used Transform. 
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    @BruceBartlett   Looks like this method will work.  I do have to make sure I select the proper body to cut for each cut feature on the machining of the casting.  Slightly kludge, but I think it will work.  It's not entirely clear from the tree what is going on with the parts, so I would worry that those invited in to review the design might not get what is constructed quickly and easily.  That it is the nice thing with derived or base parts.  Very clean.  Very obvious to all involved.  The copy part method seems a little too stealthy in my opinion.
    @Pete Yodis Onshape has been designed around part studio to be able to link parts together, once a user is clear on how to use Onshape part studio's I think this method should be clear. I also hope over time Onshape will improve the feature tree and parts list. I had this idea about clicking on a part and highlight features in the feature tree, see https://forum.onshape.com/discussion/comment/1565/#Comment_1565

    Another method I've seen work in Solidworks is to drop the the casting into an assembly and add the machining processes with cut extrudes and hole feature's. I'd like to think Onshape will have this functionality in their assemblies also in the future and could be a work around if added however I think their need's to be the ability to add parts in a part studio, I have often had the need to add an imported part into a part studio.  

    The assembly cut features in SolidWorks were limited compared to cut feature capability in part files.  I never liked to use assembly models to cut material, unless it was an assembly like feature - drilling and pinning a gear to a shaft for example.  Other than that - stick to base part insertion of the casting and then machining features.  Very clean, capable, and robust.

    Regarding the Part Studio with transform/copy part to accommodate base parts - Something needs to be done to simplify the view of which features apply to which bodies.  Right now, it would be unnecessarily complicated to invite a casting vendor into a casting and machining design and have him be a part of it.  It needs to be more simple.  I would have to give him access to the whole kit and caboodle.  I would only want him changing the casting, and not the whole casting and machining.  That is another advantage of something like base part.  It's too complicated at the moment and it doesn't need to be.  People won't naturally move to overly complicated tools.
  • fastwayjimfastwayjim Member, OS Professional, Mentor Posts: 219 PRO
    Not sure if this has been discussed yet, but I really like the ability to add draft on the fly while creating an extrusion. This saves a bunch of time for complex sketches which are being extruded, for example: Text being molded into a plastic part - this should be created with 2 features: "Sketch" & "Extrude w/ Draft".
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    I should add another item to this list... The ability to color features/surfaces differently than the global body; This is really nice for machined features on a casting; All features machined show as ;a different color on the casting; It is real obvious visually and very quickly what surfaces are being machined.
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,585 PRO
    edited March 2015
    In addition to Pete's colors, cosmetic threads created with a different face color really makes them stand out.


  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    Not sure if this has been discussed yet, but I really like the ability to add draft on the fly while creating an extrusion. This saves a bunch of time for complex sketches which are being extruded, for example: Text being molded into a plastic part - this should be created with 2 features: "Sketch" & "Extrude w/ Draft".
    That is handy for sure, but what would happen in a design when the parting line needs to change @FastwayJim ? I actually don't model the way you mention most of the time. I actually model all features as nominal, with no draft. Next the parting line is determined and split faces are created on the part to capture that. After that, draft is applied properly. After that, fillets are added. If the parting line ever needs to change based on vendor feedback, it can quickly be done under the split faces step. If all the draft is modeled on the features, then I could possibly have some rework on each feature. Its not always the case, but has worked out to be a flexible and robust method for me.
  • fastwayjimfastwayjim Member, OS Professional, Mentor Posts: 219 PRO
    Molding in text is a specific case, where I embed the draft automatically. In my experience it is added as one of the last features in the model (after all drafts and radii have been added), and it always slapped on a face normal to the pull direction (which has already been established at this point). I just HATE having to pick 30 surfaces at once...

    Granted, the draft on text is not really needed to be in the model (typically doesn't change the mass by much in plastic parts), and toolers know how to machine it properly, but I'm a stickler for details.
  • pete_yodispete_yodis OS Professional, Mentor Posts: 666 ✭✭✭
    edited March 2015
    I was reading too fast.... Yeah, text is where I would use the draft on the feature itself... You're right - it's nasty having to pick all those surfaces. I'm also a stickler on details - I like my models to reflect reality if its reasonable enough. Text is where the molders would want a fair amount of draft to make sure those small features get enough separation from the tool.
  • steven_zhusteven_zhu Member Posts: 2
    Yes, we are waiting for the tool of castings, plastics a long time
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 422
    @steven_zhu  Can you say what specific functionality you need for casting an plastic injection molded parts?

    Is this for the design of the parts for this process, or the design of the tooling for these processes, or both?
  • colemancoleman OS Professional Posts: 244 PRO
    I would be most interested in the mold design functionality.  
    Spure, gate and runner library.
    Analysis
    Library of standard mold components: leader pins, bushings, mold bases etc. 

     
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 422
    @coleman You are speaking to plastic injection mold design functionality, correct? Could spur, gate, and runner library be accomplished with derive part from a linked document? Analysis - I assume you mean mold flow? Standard parts libraries that contain pins, bushings, and bases - can list some suppliers here that you are interested in seeing?
  • colemancoleman OS Professional Posts: 244 PRO
    @PeteYodis- Yes I am referring about plastic injection mold design functionaity. 
    Sprue, gate and runner could be derived parts but maybe a different route would be better.   
    If I need to create a runner.  It would be nice to select a sketch, then in a dialogue window....define the runner parameters- shape (half round, full round, profile etc.). 
    Same for gates- Select a sketch point and then define parameters.  
    Same for sprue.....or just import the sprue bushing which would define the profile. 

    Mold flow analysis is a must to compete with our current package.  

    As far as suppliers- dme is a great start. 
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 422
    @coleman Thank you for your response here.  It sounds as if runner, gates, and sprues need a FeatureScript emphasis... ref @dave_cowden   Injection mold design is similar, yet different to perhaps metal cast tooling design - but there is probably a decent amount of overlap here.

    Thanks for the supplier reference.

    What do you use for mold flow analysis currently?


Sign In or Register to comment.