I would like to design a part in Wildfire 2.0 that is a sheetmetal tube along a sketched trejectory (bend tube for an exhaust system) that then has a formed feature embossed into it (dimple to slow the velocity). I can't figure out how to get the shape I want without using a swept protution in solid mode and I can't figure out how to get it to work in sheetmetal. This will best simulate out mfg process. (I could just make it a solid but there is no challange in that.)
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sheetmetal tube with embossment 1
- Thread starter kgrzebien
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First of all, a bent tube is not a sheetmetal part. So I dont see any benefit by making the model as sheetmetal.
Second, if you really need a feature (like a boss) on a sheetmetal surface, use the FORM option. This allows you to place and "punch" the desired shape as defined by your form feature, which is a solid part in its own.
Second, if you really need a feature (like a boss) on a sheetmetal surface, use the FORM option. This allows you to place and "punch" the desired shape as defined by your form feature, which is a solid part in its own.
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- Thread starter
- #3
Our manufacturing process stamps a dimple into the tube after bending (like a sheetmetal FORM feature). I'd like to simulate those steps in our models. I am aware that a tube is not a sheetmetal part but to the best of my knowledge you can't put a formed feature into a solids part. I'd pefer not to have to model the tube, model the dimples and then shell the part, it may look similar to the actual part but it will NOT represent the actual mfg processes.
In the past I've used a cosmetic feature to represent the features.
In the past I've used a cosmetic feature to represent the features.
Why not add the dimple as a surface (assuming it's shape is easier to make this way), then thicken the surfaces after.
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- #5
As with all of our sheetmetal parts, we design the tool that does the embossment (die or form feature) for production and use that solid model to in sheetmetal mode to form the feature desired. It's a simple and accurate way to maintain consistancy between tooling and production parts. if you use a surface feature thickened or solid model with cuts and radii etc. then shell it, you have no control of the tooling except thru personal knowledge.
telecomguy
Mechanical
You deserve a star for that. I think it's a great idea to maintain consistency between tooling and your proe library. Otherwise, the model looks great and the parts don't work. Or else, you copy a part that works great to create a new part, then find out they can't build it because they've manipulated a tool so it won't work on this new part.
As far as your modeling problem goes, I was able to do the following:
-Create a datum curve through a series of 3d points
-Create a Swept Blend along the curve with an appropriate cross-section at each datum point
-Create a datum point along the curve where I want a formed feature
-Create a datum plane through the point and perpendicular to the formed feature using an angular reference
-Create an axis through the point and perpendicular to the plane
-Insert the formed feature at an offset from the plane and aligned to the axis. I tried several ways of creating a tangency constraint when inserting the formed feature but it would not work. So I backed off and just used the radius of the pipe as an offset dimension.
Good luck,
<tg>
As far as your modeling problem goes, I was able to do the following:
-Create a datum curve through a series of 3d points
-Create a Swept Blend along the curve with an appropriate cross-section at each datum point
-Create a datum point along the curve where I want a formed feature
-Create a datum plane through the point and perpendicular to the formed feature using an angular reference
-Create an axis through the point and perpendicular to the plane
-Insert the formed feature at an offset from the plane and aligned to the axis. I tried several ways of creating a tangency constraint when inserting the formed feature but it would not work. So I backed off and just used the radius of the pipe as an offset dimension.
Good luck,
<tg>
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