Profile Milling with Tool Compensation and Ramp Entry for Internal Profile

[CRIS_AFARELLI]

Profile Milling with Tool Compensation and Ramp Entry or helical for Internal Profile

Hello CREO Users,

I am working on a milling operation for an internal profile (similar to a valve seat geometry) in Creo Manufacturing. My objective is to machine the internal contour using tool radius compensation (CUTCOM) and to ensure smooth ramp transitions between Z-level passes or using helical folling the profile to avoid marks on the final surface.

I have tried the following approaches:

• The Cut Line strategy allows helical movements and smooth transitions between passes, but it does not support tool radius compensation (CUTCOM). This is a requirement for my process.

• The Profile Milling strategy does support CUTCOM, but it does not offer ramp or spiral entry between Z-level cuts. As a result, the tool plunges vertically at each level, which causes unwanted marks and steps in the internal diameter of the part.

• I've tried to explore all the SCAN_TYPE parameters. LEAD_IN and LEAD_OUT approach but nothing works well.

I need a solution that allows:

• Internal profile milling

• Tool radius compensation (CUTCOM)

• Smooth ramp or helical transitions between Z-level passes

Is there a way to achieve this in Creo? Can you suggest any workaround or configuration that enables ramped transitions with CUTCOM enabled in Profile Milling or another equivalent strategy?

[KenFarley]

A way to maybe get what you want is through the use of an older type of toolpath

Classic NC Steps -> Custom Trajectory 

This type of toolpath is something I use a lot for crazy contour-following rougher cuts and lots of other weird geometry situations. It isn't available within the manufacturing module unless you set the hidden config.pro option

enable_classic_nc_steps yes

It is a very simplistic cutter path definition. With this you could define a path that has nice circular lead-ins and that should avoid the terrible vertical z-motion "scribe line" effect.

A helical z transition I've not seen, but would really like to. I could define a helical surface, but that's useless for machining because it won't know how to follow the surface, unless you can use the surface edge as the path? You'd have to try it, but I don't have much confidence in it...

[CRIS_AFARELLI]

Hi Ken

Thanks for the insights and suggestions.

I’d like to share that I found a workaround using the Volume Milling strategy with the PROF_ONLY option and SCAN_TYPE = SPIRAL_MAINTAIN_CUT_DIRACTION. It supports internal profile machining and by adjusting the scan type and entry/exit parameters, I was able to create smooth transitions between Z-level passes, very similar to a helical or ramp entry.

The only limitation I noticed is that CUTCOM is not applied.

Also, regarding your suggestion on the legacy toolpath: I checked my configuration, but I couldn’t find the enable_classic_nc_steps parameter in my config.pro.

The image below is the profile that I want to machine. I use a ramp angle to connect each slice, this way avoid tool marks at the internal profile.

[KenFarley]

Because the config.pro setting is hidden, it does not show up in the typical options editing interface. You have to manually add it to your config.pro with a text editor. For some reason they seem to feel that this toolpath type is not needed anymore, which I wholeheartedly disagree with. I want the level of control that this type of path provides, because I find that many of the "simple" path generation methods are lacking in some aspects.

[CRIS_AFARELLI]

Hi Ken,

Thanks again for sharing your idea with me. I really appreciate it!

I ended up finding another solution using the Volume Milling strategy with the PROF_ONLY option and SCAN_TYPE = SPIRAL, MAINTAIN_CUT_DIRECTION. It worked well for internal profile machining in this case.

That said, your suggestion regarding Custom Trajectory is still very valuable. I can definitely see its potential for other manufacturing scenarios where I need more control over the toolpath.

I’ve already edited my config.pro to enable this option. I hadn’t realized it was a hidden configuration. Thanks for pointing that out!

[bmuller]

I completely agree with the use of the trajectory tool path as a catch-all for the difficult problems. However, at least on Creo 11, I don't think I could recommend the old classic step anymore.  They seem to have completely subsumed the classic trajectory into the dashboard, unless I'm missing something. Besides being dash-board oriented, the new trajectory has tool path preview, which allows parameter changes to show up immediately, which is nice.

[KenFarley]

I don't use Creo 11. We're on Creo 9 and likely will be for a while.

I would have to see proof that I can define the types of trajectories I can do with the classic custom trajectory before I'll believe anything. I do (today, all day as a matter of fact) 3D complex surface milling paths with flat roughers where I need the toolpath to compensate its motion to avoid gouging, follow the contour with the current contact "point" of the cylinder, cut along a defined curve which ends at a point corresponding to the maximum height of the part, etc. The Creo 9 trajectory, as far as I can see, doesn't seem to allow me to sketch the path I want to take. Seems to want me to use edges, etc. The kinds of things I need to do are one of the reasons I didn't switch to doing toolpaths in MasterCAM, which would be much simpler in terms of being able to share work with colleagues, etc. I just could not get it to do the things I need to do.

[bmuller]

I hope my reply didn't come across as a criticism. I am glad you liven up the forum, and I've found your responses helpful and enlightening. I've just been using the dash board version of trajectory, and have had good results.

As an antidote to slow day boredom, I discovered the tool path shown below, so I am sort of glad I read this thread. Part of the problem with these tools is that I haven't tried out that many of the options in the drop downs and check boxes, and the manual leaves it for us to discover how to use them. I looked at version 9 trajectory and compared with 11, and they seem identical I am curious now if I could repeat some of your tool paths with the newer version. I may need to use classic trajectory if not.

I wanted to pipe up because I kind of dread running across the menu manager anymore. Sometimes I try to gather a mill volume as a puzzle to test my wits; I usually fail. 🙂

[CRIS_AFARELLI]

Hey everyone,
Just wanted to say I really appreciate the technical discussion here. I always end up learning something new, and it’s great to see different approaches being shared.

I recently enabled enable_classic_nc_steps in Creo 11, though I haven’t explored it much yet. I agree that the classic  machining strategies definitely require a bit more patience, especially when dealing with those cascading menus… it sometimes feels like navigating a maze! 😅

@bmuller  — I had a quick question about the image you posted. It looks like you’re machining a parallel diameter. Would you be able to add a chamfer at the beginning and interpolate the toolpath to machine the chamfer together with the diameter? I’m curious to see how that would work with the trajectory or other machine approach you’re using for.

[KenFarley]

I'm always worried when we switch to a new version of Creo. I'm concerned that a type of toolpath I use all the time will now be deemed "obsolete" by whoever is making the decisions about the manufacturing module.

For example, we make a lot of large electrodes with surfaces that have 10, 20, 50 or whatever surfaces that need to be machined on the working surface of the part. For decades (since the mid 1990s) we've used a surface milling toolpath with a ball mill that steps over with parallel paths. The distance between adjacent passes is calculated by the software, based upon a defined allowable scallop height. Defining toolpaths for these parts with this surface-linear passes path is extremely easy. So, when we upgraded to Creo 9, there was a general freakout because that particular type of surface mill was no longer there. You would still pick all the surfaces you wanted milled, but the paths generated were idiotic, terrible, and inferior jumps all over the place milling each individual surface one at a time. Horrible results, dopey plunges all over the place, etc. Luckily I was able to find, somehow, the now-hidden option

enable_classic_cutline yes

which returns calm and soothingly boring toolpath definition.

So, I'm always worrying that in a future release of Creo, we'll find that the "classic" types of cuts that we rely on almost every day will be eliminated altogether. 

[bmuller]

Yes! I feel your pain, because that is exactly my experience with that surface milling tool, and I was upset about it, same as you. I never thought about using that hidden option, so I went without for a long time.  Then, as luck would have it, one day I tried the button marked "cutline milling" and found out that was where  they moved it.

I think a better solution than just removing that part of the surfacing and leaving us wondering would have been to  link to the new in the surfacing menu manager. Oh well. You might try the cutline milling and see if everything is there.

[CRIS_AFARELLI]

@bmuller 

I’d like to bring this topic back into the spotlight, specifically about machining internal hole profiles.

I haven’t been getting good surface finish using the Volume Milling strategy with the PROF_ONLY option and SCAN_TYPE = SPIRAL_MAINTAIN_CUT_DIRECTION. (Please see the picture attached.) After removing the part from the machine, I had to manually improve the surface using hand tools, which obviously isn't ideal.

I also tried using Cutline Milling, but unfortunately didn’t get good results with the toolpath in this case — especially when trying to handle the transition between the angled and cylindrical regions of the hole.

Have you had any success machining this type of geometry? Or do you know any workarounds that might help improve the toolpath quality and surface finish?

Thanks in advance!

[bmuller]

Would it be reasonable to say that the problem has gone from one of software to a problem of process? If so, you might try a machining forum like https://www.cnczone.com/

or 

https://www.practicalmachinist.com/

[CRIS_AFARELLI · Accepted solution]

Hello everyone,

I’d like to share that I achieved very good results using the HSM Finish strategy - CUT_TYPE SPIRAL / FINISH_OPTION CONSTANT_Z in Creo for a complex surface profile.
The surface finish quality significantly improved compared to other approaches we had tried before.

Thanks again to those who suggested this method — it definitely made a difference.

Hope this helps others facing similar challenges!