I see one function to design Timing Screw is good
How in Creo have this function:
The fuction is not sweep or Var section sweep
This function is: Sweep with variable pitch cut from one extrude body (In creo just sweep from section, this is sweep cut from body)
Please help & discuss how to do in Creo
Thanks & Regards
If is follows a constant angle change of the "tool" it could be a variable section sweep using trajpar along a spiral guide path (origin). The path would incorporate the pitch variation, if needed, by wrapping a sketch onto the cylinder.
I have worked on a problem like this before and found that core Creo does not do this very well at all. It can do a 2D cut with ease with many options, but to remove a 3D tool, even something as simple as a ball end mill, it simply doesn't work right. I suspect you need the manufacturing extension to get this right, and even with that, I am not sure you can get this result.
This might make it clear or just muddy the waters... but if I extrude any section along Tom's model, it removes more material. This would happened continuously along the entire path.
If this can be done in core Creo without faceting the cut surface, I would love to know about it.
This is a very real condition anytime you add a mill to a rotating cylinder. Think about a grind wheel that is machining grooves into a cylinder mounted to a lathe. How would you do that?
I think this form can be generated by single point cutting. Mill out the bulk of the material and then single-point the remainder.
A flat bottom cutter won't work anyway as the the angle between the walls and the bottom changes from 90 degrees.
I will do follow step
- 1/ Make a ref point in helical curve (to get dimension to pattern) & datum plan
- 2/Cut extrude at datum plan through point ref
- 3/ Group: point, extrude, datum plan together
- 4/ Pattern folllow dimension, click dim of point
Please see the attach file & piture below
Link download files part in creo2.0:http://upfile.vn/ivQT/timing_screw.zip
However: if want to exactly, must pattern big number
Thanks & regrads
Does the angle of the flat surface need to change angles like in the video?
I did just figure out how to do a constant shape without having to pattern it by changing the sweep normals.
For instance, the see-through disk is a grinding wheel. The shaft is on a lathe.
First I sweep the section of the grind wheel along the helix, be it constant or variable; but it has an orientation along the axis instead of the origin helix.
Next, I sweep the round part of the disk; the "()" section, this time with the sketch normal to the axis of rotation (lathe).
Last, I pattern once the last sweep to provide the offset for the grinding wheel's thickness.
These 3 steps will make the part accurate as machined. I don't know how fillets may complicate this operation.
In my 1st attempt I also used a pattern method. So not satisfying
I remember leaving a "wormholed" cylinder with facets one time. It bugs me to this day.
Creo 2.0 full version attached
variable pitch (wrapped arc sketch)
see sweep section orientation for controlling the cut orientations.
This represent a grind operation. This can be adapted for other shaped... however I am still not sure how rounds will translate. The pattern method will compare the shapes for accuracy.
I know this is an old thread but I forgot about it and came up with the same solution... again.
There are some tricks to making the surface smooth when directions change, but in general, boundary blends are probably one of the cleanest solution for timing screws available today.
Here's hoping that one day PTC will have swept solid cuts available in core Creo.
This timing screw was created using a pattern of 40 instances per revolution (9 degrees). Between the non-motion to rotation of the "specimen", the 9 degrees was divided in half for a smoother transition. Once the boundary blend was created (a single feature), the surface was offset to account for the "scalloped edge" depth. The offset can also add desired clearance. The ends of the "master" were also extended to make sure the blended splines were similar in length from the start. A significant length change from spline to spline will cause other artifacts along the surface. You can still see the transition where the part starts to rotate. See if you can pick up these tips in this video:
Be sure to go to YouTube and set the video to HD.
It appears solidquirks can sweep a solid body along another solid body as a cut. something Pro/E should have been able to do long ago. You can sweep cuts in Pro/E, sure, but the geometry you get will not be what a real cutting tool will create. Sometimes it's close, sometimes not. This thread is a perfect example of why we need this. So, PTC, how about quit monkeying with the GUI and give us features we can use?
I would think that the manufacturing extension does this just fine. Problem is, we as engineers are trying to tell manufacturing what to do but not how to do it. Not allowing core Creo to create an accurate model for these processes is a huge oversight in my view. It is a rare occurrence and certainly doesn't justify buying the manufacturing extension for 99% of users. Therefore, PTC's logic puts the cart before the horse and thereby creating a communication breakdown between design intent and fabrication.
I agree. I believe WE the Designers and Engineers need to be able to 100% describe the geometry we want, and will get using a certain 3D shape (not 2D section), and that Pro/MANUFACTURING should only need to do whatever tool geometry and toolpath are needed to get that geometry. If we cannot produce the geometry we need on our end, how can we, at the asembly level, know if the geometry will work? These timing screws are being used essentially as barrel cams, so how could we accurately predict if the follower (roller follower, bottle, etc.) is able to follow the path we want?
I'd much rather be able to create the correct geometry, than have the manufacturing people have to guess what we really want.
If SW has this capability, Pro/E certainly should......and should have had it FIRST, to justify our spot on top (in price). But, hey, we DID get the ribbon instead, so.......
I recall that one can create a swept volume in the kinematics package. One should be able to create a volume as the bottle moves along the helix and perform a merge/cutout to generate the screw surface. Whether PTC has thought to allow this is something I don't know.
I remember that you can do that to check for interference, but I do not believe you can use that to remove material from a part.
I've come across instances when i needed to do this, and couldn't.