Hello all,

I am trying to model a rather complicated part exactly as it should be produced. Imagine an hour glass shaped cylinder that is machined via 4th axis with a sine wave. I can easily make this cut on a surface, but the new surfaces formed are what trouble me. I have tried surface lofts, but I lose the control of the geometry that I need. Basically, what command options do I have to make these new surfaces accurately (accounting for the geometry of the cutting tool)? If I could do a swept cut that somehow stayed perpendicular to my rotational axis, that would be great; but I don't know how to make this happen.

Thanks!
Siress

Quote:

I am trying to model a rather complicated part exactly as it should be produced.

Why? What sort of magical thing will happen if you succeed within this self-imposed arbitrary constraint?

Because of reasons.

Good day.

What you're looking for is not all that unusual. The question is often asked in the form of "can I sweep a solid?", to which the answer is no, but there are work arounds. The people who are asking this question are looking for the same thing you are: to generate a model that acurately represents what happens on the machine.
Try dropping in on this NX thread: http://www.eng-tips.com/viewthread.cfm?qid=326303
If you want some of the sample files converted to step or parasolid let me know.

Ray S
NX 7.0.1.7
www.appliedprecisionproducts.com

Actually, in SWX2012, you can sweep a solid. Look up "Sweep Property Manager" in the SWX help. I think you might just find what you are looking for.

- - -Updraft

Hi,

Why do not you post an image and maybe with math definition so that we can better help you?

Best regards,

Alex

Ray, thank you very much for your help! Sadly, the solution within Solidworks hasn't been posted in the thread you linked. I am unaware of a method that will even allow me to do a surface sweep of the tool path's rotational axis so that I can then thicken the surface.

Updraft, that's very cool, but I'm using SW2011.

Jassco, I may need to do that soon.

A picture would help to make sense what you are looking for.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

As noted - you can now sweep-cut solids (within certain limits) representing a tool following a path.
If that doesn't work perhaps this (older) technique will give you some ideas.
http://home.pct.edu/~jmather/content/DSG322/SolidW...

My point is that one should not get hung up on using machining techniques as modeling techniques. Yes, you want accurate geometry. No, you don't necessarily want to play "virtual machinist" to get it done.

Siress, the solid sweep cut goes back to SW2008 or SW2009. I use it quite extensively with SW2010 right now. As Updraft said it has it limitations and it will slow down your file, but it does work. The biggest this is to keep your toolpaths as simple as possible so it may take several features to get it done.

Quote:

My point is that one should not get hung up on using machining techniques as modeling techniques.

There are many instances where swept-solid type (or complicated techniques to replicate this geometry) is the only way to create the digital geometry. This problem posted by the OP sounds like one of these cases. Similar problems have come up on the various MCAD forums over the years.

Rollupswx, thanks for that link. I've exhausted that method prior to making this thread, though. I need more detailed control over the geometry without bogging myself down with the mathematics of a sketch wrapped onto a wavy surface. (as much as I may love Stokes' theorem)

Mncad, I've tried solid sweep cuts before, but it has never resolved a feature for me. I tried it again, following the included help file directions to the letter with defaults applied, and posted the error here. I then tried the method I actually want of keeping the tool body normal to the axis, and solidworks sat busy for 10min before I stopped it. [Note that I frequently model knurling in my parts, and that only takes a few seconds on my machine; it's not a slouch. And please reserve your judgements for applying knurling, it's because of reasons. :)] Perhaps you could direct me to a good example of someone doing what I'm attempting?

Regarding the attached, the part is a revolved spline. The cutting tool path is a 3D spline on the surface of the part (this provides me the actual geometry that I am concerned with detailing, instead of a wrap). The tool body is a simple revolved rectangle, not merged with the part, tangent to the tool path with the rotational axis of the tool body lying on the tool path.

Thank you all for your help!

• http://files.engineering.com/getfile.aspx?folder=b4b5685c-38c1-403c-9b54-5e

Hi, Siress:

It appears that you do not have control over orientation of your cutter.

Best regards,

Alex

Another solid swept cut SNAFU within Solidworks attached. This occurred when I attempted to use a surface spline as the tool path.

It worked great for a helix, which was mildly exciting.

• http://files.engineering.com/getfile.aspx?folder=d8a1f5ae-f2d6-491f-89cc-72

Quote (rollupswx)

There are many instances where swept-solid type (or complicated techniques to replicate this geometry) is the only way to create the digital geometry.

This does not appear to be one of them.

You could do this without sweeping a solid. Draw the path like you did, then make a ruled surface (normal to the solid surface), and then thicken the ruled surface. I've had good luck and sound, workable toolpaths with this technique.

With the swept solid (or "simulated toolpath"), the side surfaces of the cut are determined by the orientation of the tool, and the tool is not necessarily held normal to the cut surface.

Also, it seems a bit of a stretch to force the cut to be made by a single pass of a tool of exact size. Sloppy. With that kind of inaccuracy built into the process, taking the effort to be overly precise is pointless.

Quote (TheTick)

Draw the path like you did, then make a ruled surface (normal to the solid surface), and then thicken the ruled surface.

That actually worked on a simple cylinder, now that I knew how to do it. Thanks, TheTick!

Directions in case this comes up in a google search:

Once you have a tool path, create a line indicating the cutting tool's rotational axis that is incident to the tool path. Go to Surface-Sweep and select the tool axis as the profile and the tool path as the path, under options keep the orientation as Follow Path and change the Path Alignment Type to Direction Vector, then select a surface with an axis of symmetry the same as your part.

However, the same method applied to a wavy surface yielded the attached; which isn't close at all.

• http://files.engineering.com/getfile.aspx?folder=819bff2c-c1fa-49da-85c5-92

You don't want to make a sweep surface. I'll try breaking it down for you.

• Copy outer surface (with offset).
• Draw centerline of path on surface.
• Use Split Line to cut the surface along the path.
• Create a surface normal to the copied surface along the split line using Ruled Surface.
• Thicken the ruled surface to the tool diameter (do not merge, keep as separate solid body).
• Use Move Face --> Offset to ensure tool path body properly intersects your model.
• Subtract tool path from main solid.

Feeling generous. Made a model. Stuck w/ cylinder to keep it simple.

Note use of "spline on surface" in 3D sketch. There might be better ways, but I like this way.

• http://files.engineering.com/getfile.aspx?folder=16989bf3-5f4e-4b2d-a9a0-45

Awesome! Thank you.

I'm getting a future version error, as I'm using SW2011. I still appreciate the effort.

Hi, TheTick:

I took a look at the model you created. How do you know that the ruled surface created based on the 3D sketch (on surface spline) is normal to the cylinderical surface?

Best regards,

Alex

Quote:

How do you know that the ruled surface created based on the 3D sketch (on surface spline) is normal to the cylinderical surface?

That is how the ruled surface is defined. Check the options when creating the ruled surface. (I don't think it can be changed after creating.)

Hi, TheTick:

Thanks for the quick reply! My point is that the ruled surface has not knowledge of the cylinderical surface. When you created the ruled surface, you did not pick the surface. You only pick the 3D sketch.

Best regards,

Alex

jassco, the edge of the surface was selected, not a 3D sketch. By selecting the egdge, the surface is automatically associated.

Quote (TheTick)

http://files.engineering.com/getfile.aspx?folder=1...

Would someone be so kind as to open the file and save it as SW2011 compatible so that I may view it?

Here you go. It is a dumb solid since there is no Save As to an older version in SolidWorks (or any 3D parametric solid modeler).

Cheers,

Anna Wood
SW2011 SP5, Windows 7 x64
http://www.renderbay.com
http://www.solidmuse.com
http://www.phxswug.com

• http://files.engineering.com/getfile.aspx?folder=e2d62735-bca2-4da6-8810-af