Corner slowdowns...

[William Grizwald]

In MCX - Mill Contour...

 

Where is the setting for "slow down (either percentage or actual values) in corners"? I have a bunch of toolpaths that need to have the facemill slow down in corners.

 

I'm sure it's a simple setting right?

 

Thanks.

--

Bill

[Bruce Caulley]

Look in feed in the control definition.

[HEAVY METAL]

do most of you have this box ticked

[William Grizwald]

Bruce,

 

Yes, found it. Thanks for the help. That said, I really don't want to set all my programs output to corner slow downs. Just the face mills.

 

I was hoping to do it on an operation by operation decision. It really should be tied to the operation. My previous system had this ability. You would go into the operation and select Corner Control (you could define what was a corner by the angle of the two paths), tell it percentage of the tool dia to slow down and if you wanted it to slow down in steps or all at once. For now, I guess I'll have to break up the geometry and use Change At Point...

 

--

Bill

[Guest]

Toolpath editor is the ONLY way you're going to control 1 tool like that

[gcode]

Corner control by operation is something that needs to be added to Mastercam. All the so called "high end" cam systems have it.

Mastercam need to add this to the toolbox.

This is especially true with the advent of

high speed tool paths, but even simple contours

need the ability to control the feed rate coming into coners.

You can do it with the Toolpath Editor, but it is

a lot of work and totaly impractical for large

toolpaths.

[b_daddy]

If you look on their latest " News Flash" it shows a picture of just the very same thing that is being discussed, but after watching the video they are talking about something different than the picture shows.

[William Grizwald]

Gcode,

 

+1...

 

I have 150+ operations with various 4-5" facemills doing 800 sfm at times in cast iron. The machine load is 60-70% on straights, >100% corners. The control alarms at 105%. We load multiple parts unattended over night and weekends. So yes, I need this feature.

 

Slight side note:

You mentioned "the so called high end systems" have this feature. I won't say the name of the system I used as it wouldn't be appropriate in this forum but... The one I used actually cost a little less than MCX combined with Solidworks (which is the comparison in features IMHO). So, at that price point I expect to have this kind of toolpath control and more.

 

That all said, there's a workaround for everything .

 

--

Bill

[Rick Henrickson 65]

the answer is adaptive control on the machine tool!

[Bruce Caulley]

I agree that it needs to be an option for individual toolpaths. It also has the annoying feature of slowing down on external corners.

 

Bruce

[Guest]

Wouldn't the G8 look ahead, available on many controls, help here?

[Thad]

Bill,

 

What was your old system? It's not a big deal to mention another software, really. If you search, you'll see that people have asked questions on SolidWorks, Autocad, UG, Catia, etc here...and have gotten help.

 

quote:

---

Look in feed in the control definition.

---

quote:

---

Yes, found it. Thanks for the help. That said, I really don't want to set all my programs output to corner slow downs. Just the face mills.

---

I'm not sure what setting you're referring to, but maybe this thread will give you some ideas.

 

Thad

[cadcam]

Have you guys tried change at a point in the Geo tap?

But the toolpathe editor does a easer and faster job.

[William Grizwald]

Thad,

 

Like I said, I feel it's not appropriate to discuss comparisons (this is a very passionate group...) I will however focus on needs for features I'm used to and would benifit MCX.

 

Jay,

 

Like Gcode said, it should be a switch in the operation. There is no better way to do it.

Toolpath edit and At Point are not the best place when you work in a revision changing environment.

It's also way more obvious to other programmers who may have to work with someone elses file.

 

What I'm finding is other programmers (in a hurry and lacking patience) just run the tools based on the worst case corner load - which is unfortunate.

 

--

Bill

[New Job]

Is there a c-hook (or other third party software) that would be available to apply these type of changes to the posted toolpath?

[Scott B]

Did you look at the "High feed" option in the operation manager. It is located next to the "G1" post icon. This might be what you are looking for.

[William Grizwald]

"Did you look at the "High feed" option in the operation manager. It is located next to the "G1" post icon. This might be what you are looking for."

 

I checked that out. Looks interesting for perhaps global editing of parameters. But for not for my needs, I just want a simple corner control switch. Being a newer user I'm shocked it has not been in MC for years now, it's a very common requirement for proper milling.

 

--

Bill

[Guest CNC Apps Guy 1]

quote:

---

...I feel it's not appropriate to discuss comparisons...

---

Comparisons ARE great. Lately I ripped into CATIA, and at the same time, scolded Mastercam. Just be respectful is the pain theme.

[mike rosa from cnc software inc.]

William,

Highfeed will do exactly what you want and it's been in our software since V7. Define your machine dynamics in the general machining parameters including Max. feedrate change per block, Minumum cornering feedrate, and angular direction change. Select desired toolpath(s) to modify corner feedrates and run Highfeed Finish Only. You can edit the local copy of your machine definition to quickly change the highfeed values if different parameters for other toolpaths apply.

Highfeed can also be used in your roughing operations. As you, or someone else mentioned, a program is generated for the worse case scenario. Full width and depth of the tool. This condition occurs a small percentage of the time in the program but must be accounted for. Whenever these conditions improve, for instance, stepping over 45%, the feedrates can increase. Highfeed will adjust the feedrates based on the volume of material being removed, changes in direction as well as take into account machine dynamics to prevent overtravel.

 

You can contact you local Mastercam dealer or me if you have any questions or problems.

 

Mike Rosa

CNC Software

[email protected]

[gcode]

mike,

high feed does work, but can be very cumbersome to implement and it has one huge drawback. It will not properly post toolpaths that are using cutter comp. (if this has been fixed for X2... my apoligies)

This makes it nearly useless for my needs

In my view every contour and pocket operation need the ability to control cornering feedrates.

 

Another very high tech option would be the ability to define feedrate as feed per tooth

at the periphery of the cutter.

 

This is essential to getting good insert life with modern insert mill technology and Mastercam needs to be able to do it.

[William Grizwald]

"mike,

high feed does work, but can be very cumbersome to implement and it has one huge drawback. It will not properly post toolpaths that are using cutter comp. (if this has been fixed for X2... my apoligies)

This makes it nearly useless for my needs

In my view every contour and pocket operation need the ability to control cornering feedrates.

 

Another very high tech option would be the ability to define feedrate as feed per tooth

at the periphery of the cutter.

 

This is essential to getting good insert life with modern insert mill technology and Mastercam needs to be able to do it."

 

Gcode, you hit the nail on the head. I just wanted a simple setting. I don't need an all encompassing feature to deal with. That said, we can say the issue is resolved and move on to bigger fish to fry.

 

+100 on the feed per tooth! Some systems have boxs for SFM and FTP right next to Speed and feed.

 

--

Bill

[William Grizwald]

Mike,

 

"Highfeed will do exactly what you want and it's been in our software since V7. Define your machine dynamics in the general machining parameters..."

 

OK. Thanks.

 

--

Bill

[3R!< W3NG3R]

I agree with gcode, there should be a simpler way then using highfeed (which I don't like too much)

that said, maybe thay will include it in a future releise (next one???) along with the many other features I feel they need to catch up on.