Good day! what would be the best way to this fillet. those are two separate parts. I understand its probably possible by creating another body with reverce fillet and then using it as a negative to cut a way at the part, but i was wiobdering if there is a way of doing it so the orginal fillet contols the size on the other part so they are uniform?
Hi! It is an unusal modeling technique to use blend edges to drive geometry in another component. If this is what your teacher taught you, please ask him in what industrial application this practice is followed. Blend/fillet is a process of rounding sharp edges near the end of geometry modeling. They rarely help define geomegry.
Regardless, just for academic study purpose, there are mulitple ways to fulfill your request in Inventor. I have attached two examples: Adaptive (in context) and Derive (consistent coordinate system/skeletal modeling). Take a look and let me know if you have any question.
Thanks!
THank you JDMather, your model is shapped correctly, but i am not sure its be fully applicable to my actual model (its my ar15 to boltgun gunsmithing course project) johnsonshie thank you for the models but there are dimensions that i can not change, as much of the "footprint" better stay the same, as well as for the simplisity of manufacturing the sides better remain flat. Firearm industry is understandably secretive and its hard to get information even on the basic thing.s Most common ar recievers are made form forgings with this area already formed and there are no blue prints available for those forgings to refernce from. Some other are fully machined from billet and differ from one another, and getting prints form anyone is also hard. but from what i reserched they usually use "corner rounding end mill" if the parts are machine from billets. I wanted this fillet dimention be changable in one place to simplify the refining process in the future if case its not gonna go well the first time and just curiousity sake. Sorry i dont have engeniering back ground some machining, learned inventor on youtube and here =). I wondering if there is a way to "extend" the round surface on the top part so it can cut way at the bottom part. I know its posible with in one part jsut not sure how to do it with in the assembly.
Best Regards!
thats the actual part
Here's another way of doing. It seems good for late changes in complicated parts.
Walter
Walter Holzwarth
sorry just a quick question how did you selected reference surface to extend, when i do it it gives me this, i am in the part mode not and assebly?
Try this:
- Open your iam
- Edit (in iam) Part1
- Copy object (Option surface) one of filleted surfaces of Part2. Select surface as new element.
- Extend the vertical edge of the surface for a certain amount. Value must be great enough, but doesn't matter
- Thicken this extended surface (1 mm outside) with option cut. It takes too much material
- After doing this, close the remaining groove by Face delete with healing
Do the same procedure for the other surface, or simply split Part1 in symmetry plane, and mirror it (Option body)
Walter Holzwarth
