I am new to solid works. I can't figure out how to loft or sweep in between the shapes contained.
What is the right way to connect two profiles. The profiles I desire to connect should be clear in the attached file.
Loft boss od, loft cut id.
Loft Feature requires just two profiles, which in your case would be the outside shapes. Edit the sketch and make the inside lines Construction Lines..
Don't need construction line.
Just pick od loft boss.
Reuse sketch for id loft cut.
Make sure select close loop on the slot:
There's no need to edit the profile sketches. Just use the outside loops for the Loft and the inside ones for the Lofted Cut.
So I need 4 sketches to get it done. Both ends of a Loft/boss, and Both ends of a Loft Cut?
2 sketches, 4 profiles.
Pick od in one sketch, pick od on another sketch. Loft.
Expand the loft, make sketches visible.
Repeat for id.
But once I make the ID's construction, cant use them to cut. Have to have 4 sketches as a result. It is cutting the inside I have having a difficult time with now.
You could, I did.
Expand the loft, show the sketches.
Make them visible.
Construct OD first then cut ID.
Here is what I did:
Create 2 sketches and convert entities on the outside edges of the boundary
Create a fully solid boundary feature (I used boundary rather than loft because in my experience it is more robust).
(make sure you position your guide line to minimize twist or add more guide lines)
Then created a boundary cut using the inner faces that were left. Again, position your guide line to minimize twist.
I didn't even use sketches for the boundary cut (see my reply). Just used the faces that were left after the boundary boss feature.
S. Leacox wrote: But once I make the ID's construction, cant use them to cut. Have to have 4 sketches as a result. It is cutting the inside I have having a difficult time with now.
S. Leacox wrote:
Don't make the ID's construction. Use the same sketches for both features. Did you look at the screenshot and model I posted above?
Since your oblong slot shape & circle shape are extruded, no draft or curve or angles going on, using a sketch for the circle and a sketch for the oblong profile is OK as you can set their condition to "normal to profile" (perpendicular to the sketch plane for those profiles), which in this case is the same as tangent to surface that the sketch is located at (the exterior of those 2 bodies).
My preference for something like this is not to use sketches for those profiles, either select the model edge for the outside profile on each body, or select the planar face at that location, then set tangent to surface for both. Selecting the faces is the easiest in this condition.
One other thing I've noticed or suggest, is if you want to end up with this being a tube form throughout, just model the whole thing as a solid rod so to speak, then shell it to your desired thickness at the end. To do a loft/boundary cut on the portion that blends the 2 bodies together is more work and effort, often it may not be just right either in wall thickness or in it's blending, it's just much easier and more robust to shell after your outer form is completed.
You could choose not to merge the blended portion, then shell it to match the other 2 body thickness, then combine the bodies together, which works, is more steps and effort along the way, and sometimes may not blend well to the other bodies while maintaining the wall thickness. Make sure those blue ball indicators by the profiles are located at the same position/height or the feature ends up twisting.
Great info, thanks for all the help. I should be able to get back on that design project within a day or so. I will give some of this a try. Over 500 new parts to make in my design Que.
95% of my work is sheet metal. This is a non typical design of a 3/4" sch40 pipe that is crushed at the ends. Was trying to use an obround with about the same perimeter as the pipe for a first approximation. was planning on dialing in the interior cutout to near 0 width.
I was expecting a few to suggest making it all one sweep with a bunch of cross sections.
I have never used the shell feature of works. That will be a new workflow for me. I come from a background of reverse engineering from laser scans,AutoCAD and Solid Edge.
In real life, it get's flattened to thinner than two wall thickness
I was hoping for the following qualities in the finished model:
1. variable driven. Was hoping to be able to edit the over all size, OD, ID, flattened section, length of transition etc after the model is complete. This become a "Template" for any pipe that had flattened ends and two 90 deg bends. To put this another way, A seed file for designing easy to manufacture handles. So I don't care how difficult it is to make the first time, as long as it works, can be modified, and facilitates a draft showing the finished outside dimensions.
2. Dial in the flattened part after we make a few to represent exactly what it looks like after testing a few different machines for the flattening step. A uniform thickness is not desired in the flattened/transition section. I could care less what the transition looks like for thickness other than being a decent approximation of weight and someday strength in FEA.
Because of those issues, I never use shelling methods. The extra work to connected to parts is the way I would like to work.
i am curious about if this model could be precisely manufactured in real plant.
Well, in my model, I didn't check to make sure that the perimeter of the circular portion matched the perimeter of the oblong portion. If I were doing this for work, I would be making sure that they matched. Except for that, I don't see why not.
Yes this is easy to manufacture. That is the reason I am trying to make this model. CAD is much more difficult than the real operation if you have the tooling
Taking note of your comment of this being a metal with one end smashed flat, the oblong end, maybe model it slightly different from my previous way. When you model the oblong, model it as a solid if not already, as it's thinner than the 2 walls of metal present due to being smashed flat. Model the loft or boundary blending between the round and oblong bodies, as a solid, not hollow still. The change is to only merge this to the round body and don't merge it to the oblong body. Shell out both ends of this round/blend body, then combine it to the smashed oblong body.
..I'll fish,.. how I may attempt this..
I decided not to go that way because I did not want to fight the battle of moving from an open to closed shape. Kinda like Hems where the radius is not 0, just very small.
i have to say you are really talented.
your attach i could not open
I converted your part file into a parametric design and added calculations to ensure the Outer path length of the flattened tube matches the round tube.
I copied your original sketch and made it "Master Sketch" with all dimensions controlled by Global Variables. Then the feature-specific sketches use Convert Entities so that they will update automatically. I like to rename features to remind me what I am doing!
I set up new planes for the Round & Flatten profiles so that they can be re-used for the Transition. Note all features are done with just 1 Master Sketch, 1 Path sketch and 2 Profile sketches.
Transition uses Loft extrude & Loft cut method. Did one side with separate bodies, then mirrored & combined. This way you can add holes to the flat part before mirroring.
I set up formulas to calculate the circumference of the Round pipe, then adjust Flatten Height to ensure the circumference of the Flat Tube matches Round Tube.
Now, to do any other handle size, just edit the numbers in the Equations dialogue. Make sure to specify "configuration specific" and you can add configurations for each new size, as needed. Or set up an Excel Design Table to add many sizes at once.
Thanks Jacky.. btw, not sure why you can not open,.. I tested/download the above zip, no problem?
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