I want to make a cylinder, and it has a hollow inner spiral. I can make a hollow inner spiral,but how can I make it inserted in a cylinder.
The picture shows a object, but it doesn't satisfy my requirement.I need a hollow inner spiral.
If I understand correctly, you want to intersect the cylinder with the spiral tube. What does the section look like if it is the way you want?
Right now you show IO OI If you want a different section, you need to create it with a more appropriate sketch. You can also merge surfaces.
If you can, please post a picture of what you want the final part to look like.
Not enough info to help you. Do you want a helical coil inside a cylinder? As in some sort of heating or cooling coil inside of a vessel?
Yes, A solid cylinder inserted with a hollow helical coil.The picture shows the intersection of the coil and the cylinder is solid, I want to remove the material. Also, I want to merge the surface.
Actual I want to do this.The picture below is a coarse diagram. The black line represents a solid block, like the cylinder. The pink line represent a helical hole. It firstly spirals up then it spiral down.
I can mkae a helical coil surface, but how do I inerset it into the cylinder, and how to merge the surface in the bottom line.
You can create spirals independently and then create a sweep feature from the ends to the cylinder bottom. You can merge the faces several ways, but a simple method is to create Fill feature. If you do all this as surfaces, you can Merge all these surfaces into a quilt. Once it is one big quilt, you should have the Solidify feature available to make this a solid mass.
if this is what you are asking,please check,i made just rough one.you can get an idea how to do it.
(chain references 1 and 2 are no necessary,you will see them in feature tree)
Thank you very much for your kind help! But is it a version or some else problems? Why I can't open the file in my pro/e , my pro/e is wildfire 4.0.
I do not have WF4 loaded but I did attach a STEP file that you can import. I also created the following video showing how this part was made.
It was my option to make the entire unit with surfaces and then thicken the surfaces to make it a solid.
You could just as easily make the solid from the beginning. There is no -right- way.
Also, normally, the coils and the chamber would be created separately and assembled in an assembly file.
Do not try to carry one of there through the airport or onto a plane; you might end up in jail ...or worse!
Hi, Antonius Dirriwachter, thank you. But I'm sorry to tell you that, I'm from China, so I don't have access to youtube. Can you send me the video through the e-mail. I'm a little hurry for this. - or firstname.lastname@example.org
I'm a student, what I'm doing is a holmthz coil, just for the medical resrearch.
I know you are a nice guy. If possible, can you tell me how to merge the end sides of the two hollow coils smoothly in the left side of the picture below. To make them connect, I tried some methods to connect the two ends, but it doesn't work. Thanks in advance.
It is recommended that you create a sketch so a sweep feature can be created. The important part of this sketch is to be normal to the face of the opening.
You can do this several ways but I recommend creating a short line into the opening by making 2 datum planes; one on the opening face, and the second normal to the new plane -and- two vertexes on the opening. Use the data you already know to create a line in the center of the opening -into- the tube.
Next, create a datum curve through points and select the ends of the two lines you will have sketched, one into each end. Set the ends of the datum curve to be tangent to the two lines. Then you can tweak the curve to make a smoother radius (part of the datum curve dialog).
Next, use the sweep tool to create the connecting tube. The trajectory is the datum curve, and the sketch is a project of the end of the tube.
If you did all this correctly, the sweep feature will be tangent and normal to the coils on both ends.
This is a very common procedure for Creo and WF users.
Because I had good control of the ends of the coil, I was able to do this with a simpler sketch. The dashed line is to control the angle of the end of the tube given the center, diameter, and pitch. I knew the connecting sweep would be tangent and normal using this method.
The suggestion above is like this:
For the sake of completeness, I should add this method for creating 3D curves.
The following is created using 2 sketches, again, to create tangency/normal to the spiral tube (green edges of the surface).
These sketches are curved for cosmetic reasons but they are slightly different as the tangent for the inside coil is different than the outside coil.
The two sketches are joined with a simple Boundary Surface feature.
A Sketch with an arc is projected onto the Boundary Surface.
The resulting curve from the Project feature is used as a guide for the Sweep feature.
This method provides more precise control of the resulting curve compared to the datum curve through points when the point set is limited.
Feel free to interrogate the attached file if you have Creo 2.0 parametric, full version.
Also included is a STEP file for all other platforms.
i have used datum curves,just want to know if it is a bad practice.
sections and profiles appear expanded for every feature on a model tree.like in catia model tree,is that new thing in creo or different model tree settings?
Nothing wrong with creating datum curves. It is the easiest way to create 3D curves. They are simply another sketch. You want to manage them appropriately from a visibility standpoint so they don't mess up your drawings.
I opened all the features manually. No magic buttons for that
you solution is much elegant and easy to represent on drawing.
there is something fishy about your model tree,in pro/e helical sweep won't show its children.
You are right; the old model manager commands don't share their children, but the revamped ribbon features do.
There is still a lot of disparity in what you can and cannot RMB-Edit in the model tree. It is still very inconsistent.
I am hopeful that Creo 3.0 will iron all this out but it might also mean we loose some of our beloved model manager features to a consolidated ribbon feature.
I still need to share my technique of using ribbon surfaces to create coils with transitional geometry. I always use ribbons (even before they were called that) to create the basis of my coils. This gives you great flexibility when transitioning in and out of the coil. You can use things like surface rounds and boundary blends to complete the transitions. Finally, you use the edge of your ribbon as the trajectory for the coil sweep.
This seems similar to your technique. When I have time (haha) I need to go back through this thread and examine what you've done. Nice work!
Those weren't the ribbons I was referring to but your right. There are still significant limitations to making a good continuity paths.
I didn't much like the ribbon feature. it was cryptic and failed more than it was successful. Of course, that is at the hands of a novice with regard to this feature.
Holy Etch-A-Sketch Batman! Sounds like you're trying to do a set of cooling tubes in a cooling and/or pressure vessel. I saw a large, very cool example of the core of one the other day on a flatbed truck. Without knowing exactly the configuration you need, it's kind of hard to help. I think "ptc-4684141" has a pretty good pic of what you sketched. What I will say is with only 2 coils, the density of the cooling tubes isn't optimized for the interrior of the vessel. I'd do 6 or more, or do a completely different configuration, such as concentric helical coils, alternating direction for each "ring"