Hello Guys!
Im completing one quite big assembly (ca. 200 parts) and even with all the research around forums I cannot find a solution to solve a problem with bending following channel:
I have left only tow bendings of part with radius R400 and R180, but i think that i don't know how to use it properly. I cannot figure out how bend should be made:
Can anyone help?
Thank You in advance
Hello Samuel, there is quite a lot to understand about the flex feature. Perhaps the following will help. The key is to understand how to place the triad.
SolidWorks Webcast: Episode 13 — Spanner Product Development
Thanks Mark,
I haven't seen this video.
Samuel,
Another way to do this part would be to use two intersecting surfaces to create an INTERSECT CURVE. Then sweep the profile of the channel along the curve.
Look in Tools : Sketch Tools : Intersection curve
Samuel,
Edit: Yes Flex is an awesome tool but as Mark said tricky to use on multiple areas. below is a good way that is simple and less intrusive to an assembly.
this is easy when you use 2 bodies and the combine tool - common option.
as keith kind of did, draw your finish sketches one on the top plane and the other on the front, extrude the first and then extrude the second but deselect the merge bodies box, the select the combine tool, check the common circle, then finish, then shell to get the wall thickness.
You don't must make surfaces
1. create two sketches
2. Use menu Insert>Curves>Projected
Result: Curve 3D
3. Now use Sweep
Hi,
Intersection of two curve is okay, but it's also possible just to project to curves over another.
This one is from archive, from the year 2004:
Hello Guys!,
Thank You for all the help. I've used @Krzysztof Szpakowski proposition and it worked percefctly.
Cheers!
Projected curve of two sketches ≡ Intersection curve of two surfaces
Maha Nadarasa wrote:
Projected curve of two sketches ≡ Intersection curve of two surfaces
But less clicking...
Samuel Szulc wrote:
Hello Guys!,
Thank You for all the help. I've used @Krzysztof Szpakowski proposition and it worked percefctly.
Cheers!
Good job Samuel!
Samuel Szulc wrote:
Hello Guys!,
Thank You for all the help. I've used @Krzysztof Szpakowski proposition and it worked percefctly.
Cheers!
Nice job.
projected sketches and sweeps have there place but here are some things to think about....
Now make a drawing of it and see if you can match the drawing you used to create the part.
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
Another consideration is thinking down the road, will this be a one and done or could it be modified later by you or someone else? If not you, simple sketches and extrudes are always a better solution , KISS (acronym).
JMO, Have my instructor, Prototype\Model maker hat on.
lenny
Hi,
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
I agree.
In this case I would try to integrate all dimension is the 2 "master" sketches, on wich the path is based.
And the insert these dims as model items...
Heiko Sohnholz wrote:
Hi,
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
I agree.
In this case I would try to integrate all dimension is the 2 "master" sketches, on wich the path is based.
And the insert these dims as model items...
That's exactly what I did and i also dropped in pics on the 2 planes as a quick way as not needing to look at the print, right there in your face.
Lenny Bucholz wrote:
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
It is a big problem I encounter frequently. Specially if are making an organic shapes and want to hide hard edges of the model, using Fit Spline convert the line into spline.
Maha Nadarasa wrote:
Lenny Bucholz wrote:
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
It is a big problem I encounter frequently. Specially if are making an organic shapes and want to hide hard edges of the model, using Fit Spline convert the line into spline.
Yep you are correct, man I do this alot too!
Lenny Bucholz wrote:
Samuel Szulc wrote:
Hello Guys!,
Thank You for all the help. I've used @Krzysztof Szpakowski proposition and it worked percefctly.
Cheers!
Nice job.
projected sketches and sweeps have there place but here are some things to think about....
Now make a drawing of it and see if you can match the drawing you used to create the part.
I only suggest this because you may not be able to extract the needed dimensions because all the edges are now splines.
Another consideration is thinking down the road, will this be a one and done or could it be modified later by you or someone else? If not you, simple sketches and extrudes are always a better solution , KISS (acronym).
JMO, Have my instructor, Prototype\Model maker hat on.
lenny
For dimensioning you can use original sketches
File? In my view it is easy to make a sketch bend rather than using flex to bend the part.