When to add draft, etc.

dan_engerer

Hello. I have an engineering workflow question. As designers, DFM (design for manufacturing) should permeate the entire design process, not just being saved until the end. That being said, I'm wondering when it is best to add draft to a part. Generally speaking, these manufacturing features are a bit of a distraction from the actual part design, and they're usually left until the end. Naturally, this can cause huge problems, such as breaking mates, etc. all at the last minute.

At the same time, I'd imagine that adding draft early on in the part design has the potential to clutter up a feature tree very quickly. It's also annoying to click on a feature only to see that you've clicked on the "draft" instead of the "extrude" itself - making modifications more time consuming as you find the original feature. 

Just curious how the rest of you work, as I'm trying to set up a good engineering workflow. 

Thanks,

michael_mcclain

In my workflow i usually add draft, fillet, and chamfer at the end of the feature tree of a part. These functions consume IDs of faces, edges, vertexes and will change or create new reference IDs on your geometry. It is better to work with the original IDs and to set up your references as one to many vs many to many.

If you have an extruded cube and you reference an edge ID after a draft feature you are referencing the draft feature's new edge ID and not the extrude feature's. You are more likely to delete or modify the draft before you would modify the extrude hence the original edge ID is stronger than the post-draft edge ID which has been changed. I also avoid using a draft inside the extrude feature since a draft in a new feature can be more easily controlled and modified.

Having stronger references in the Part Studio vs assembly is a better trade-off since an issue in a Part Studio can grow much larger when it affects multiple assemblies. You can fix a few mates in an assembly more easily than you can fix an issue in a Part Studio which is referenced in many places.

As I learned in the Onshape Bootcamp it is best to reference cylindrical faces over planar faces since their geometry can be modified less often. They are not perfect, but it's advised to use them over planar faces when possible. These location selections can help mitigate the issue of missing or consumed references.

lana

An ability to create a mate connector in Part Studio at the point in history when you have the most stable references might be useful here.

mahir

You can add mate connectors in the part studio as necessary. Even if the mate connector fails after inserting draft, the mates themselves shouldn't fail. In my opinion, fixing individual mate connector references at the part studio level is still easier than fixing mates.

billy2

Like @michael_mcclain I tend to add draft to features that allow draft but I don't dwell on building a part that can be molded. The design will change to much to warrant this detail too early on. Typically, you need to get something out so people can hold it and look at it. I value getting something done vs. getting it moldable in the beginning. 

Getting the parting line correct is very important because changing it at the end tends to create a mess. Focus on the parting line, slides, inserts and how the mold will function. Design around these concepts and talk with your molder to make sure you're not doing something crazy. Not all tool makers build the same way, so have a conversation with them.

Eventually you need a moldable part and good planning is always a great practice. You will have to traverse your feature tree from beginning to end fixing your model. There's no escaping this. This is what the best designers do. It's part of the process.

For my last pass when finalizing a moldable design, I'll go through the feature list one by one and clean up the model. The better designers require the least amount of change in the end and converge on the solution sooner. No one can get it done in the 1st pass unless it's a really simple design.

As far as breaking mates, I usually mate by coordinates or in OS use a mate connector. Most my plastic parts in OS start with a mate connector at the origin. Hopefully your 1st feature won't fail.