X9 issues

[gcode]

 

If you have a 1/2" hole 2" deep and cut it with a 3/8 tool why even do a multi depth cut? Why not just helix all the way to the bottom...on size...climbing......the tool is going to push off due to the physics of the cut...the hole is going to be .005 small...if not on the very first hole with a brand new endmill...but very soon....I been doing this 20 years I know...
Then copy paste turn off ramp and you have your finish toolpath to take out the pushoff...all with no thought process what so ever.... you already have a arc lead in and lead out on your helix ramp....

 

Murlin, X9 Circlemill/helix bore can do exactly this, with one toolpath

[Müřlıń®]

Murlin, X9 Circlemill/helix bore can do exactly this, with one toolpath

Now that IS cool....

[BBprecise]

To skip long story see to Cliff notes below .

I 1st used MC in late '96 on version 5.5 (on windows 3.11) so I've used a lot of different versions over the years. I could tell you stories about me hating new functions. I haven't been programming continuous since then as I've gone back to running machines on and off, but I would say I've used 11 different flavors of MC. I also find myself using the same old toolpaths to do everything, but the guys here have gotten me looking at new ways to do the same old thing esp. JParis who I 1st met when he worked for S4A our reseller. A lot of my problems when I 1st started using X was myself not doing things correctly although the way I was doing them was how it was done in previous versions. Just like Windows (remember the old BSOD), CNC changed how things worked/functioned so they could improve/add other functions. I know the whole if it ain't broke don't fix it routine (which I still spout out once in a while), but I believe that if CNC didn't change things we wouldn't have any of the new toolpaths and we'd still be using ver.9 menu or even better pre v.7 when your toolpath operation wasn't associated with your geometry. I've yet had X9 crash my system (only had it for a month) but X7 would send it south once a week or so. It's like Win7 compared to '98, '98 was good, but boy did it crash often and it was common practice to re-install it once a year (I did same with XP as well). Win7 has been the best, most stable O/S I've seen since 3.x which had very few functions so there wasn't much to muck up the system.

 

Cliff notes:

I still use contour for 90% of my toolpaths and I can do a lot with them, but once you learn how to correctly use new toolpaths you'll realize you're missing out on a lot. I don't do any 5 axis and very little 4 axis so I can't say anything about them, but the only big problem I have with X9 is I have dual screens with diff. resolutions and MC won't maximize to full screen from taskbar. Every software has issues.

[guitar]

create/points/segment (by length or number of points)

window pick the points

done

Yes, many more steps. Plus if you must change the pitch, you must start over, instead of changing 1 variable in wirepaths. Kinda silly huh? I knew some genius was going to say that. lol

[guitar]

whats circle mill...lol

 

never found a need for it....never used it...ever...

 

Contour ramp is much easier....copy paste.....turn off ramp and you have your finish size for cc hole adjustments...linking already set...no need to figure out what size circle you want....just chain...

 

 

You just proved my point. Circle mill paths are next to useless.

[JoshC]

wow people still use Circle Mill. I mean its there but you don't have to use it. Dynamic does it way better, get with the times people!

[gcode]

Yes, many more steps. Plus if you must change the pitch, you must start over, instead of changing 1 variable in wirepaths. Kinda silly huh? I knew some genius was going to say that. lol

won't make that mistake again

[Colin Gilchrist]

wow people still use Circle Mill. I mean its there but you don't have to use it. Dynamic does it way better, get with the times people!

 

Really Josh? Circle Mill has options to rough in a "HSM" style, and also Semi-Finish and Finish a hole (using Cutter Comp), in a single toolpath. Mastercam has been making improvements to Circle Mill for the last several releases. For cutting round holes, it is far superior to the Dynamic Paths, just for the simple reason that you can rough and finish with the same toolpath.

 

The Dynamic paths are awesome, but they are roughing only. (Well, the line is getting blurred a little bit with Dynamic Contour, but still)

 

Plus, try machining a counterbore with the Dynamic Paths. Yes, you can do it, but I prefer to use Circle Mill, since I know it will plunge in the exact center of my hole, rough with "hsm dynamic style", and then Semi-Finish/Finish the hole using cutter compensation.

[JoshC]

Really Josh? Circle Mill has options to rough in a "HSM" style, and also Semi-Finish and Finish a hole (using Cutter Comp), in a single toolpath. Mastercam has been making improvements to Circle Mill for the last several releases. For cutting round holes, it is far superior to the Dynamic Paths, just for the simple reason that you can rough and finish with the same toolpath.

 

The Dynamic paths are awesome, but they are roughing only. (Well, the line is getting blurred a little bit with Dynamic Contour, but still)

 

Plus, try machining a counterbore with the Dynamic Paths. Yes, you can do it, but I prefer to use Circle Mill, since I know it will plunge in the exact center of my hole, rough with "hsm dynamic style", and then Semi-Finish/Finish the hole using cutter compensation.

Oh, I guess i overlooked the finishing options. Good call Colin i see your point. I'm a big fan of finishing my parts with different tools than what was used to rough but i guess if you are using the same tool that would be easier than using 2 toolpaths. and on a side note, using air regions we can get dynamic to plunge into a pre-drilled hole with ease, so C-bores are simple as well

[Colin Gilchrist]

I do like being able to use the Air Regions to avoid cutting material in the center of the hole, so I agree on that point. I just find that Circle Mill is great for milling holes, since you have options to actually plunge in the exact center of the hole, and you get the ability to rough using a couple of options (either spiral out with "roughing", or circle out, using "transitions" to step between radial cuts). Then there are Semi-Finish, and Finish options, that let you apply different speeds and feeds, and let you use proper compensation (wear, with line/arc lead in/out). This is awesome for interpolating holes to size, since you get compensation (which you don't get on any of the Dynamic paths).

 

Even if you want to rough and finish with separate tools, using Circle Mill still provides some advantages. If you use Dynamic to rough, and Contour to finish, you've got two totally different toolpaths to setup. If you program the first operation with Circle Mill instead, just activate "stock to leave" in XY and Z, and only use the roughing options. Then copy/paste the operation, activate your finish operations, and turn off the roughing. The toolpath is optimized for cutting holes, and it does it exceptionally well, now that these different options are available inside the toolpath.

[Colin Gilchrist]

Plus, if you use Circle Mill, and know how to edit your post processor, then you can make the post spit out G12/G13 canned cycles. You can do this with a "Custom Drill Cycle", but then you don't get Backplot/Verify for the toolpath. So by using Circle Mill with some Post edits, you can get a single G12/G13 line that cuts the entire hole complete.

[guitar]

Plus, if you use Circle Mill, and know how to edit your post processor, then you can make the post spit out G12/G13 canned cycles. You can do this with a "Custom Drill Cycle", but then you don't get Backplot/Verify for the toolpath. So by using Circle Mill with some Post edits, you can get a single G12/G13 line that cuts the entire hole complete.

 

Why would you want to?

[Colin Gilchrist]

Why would you want to?

 

Some of my customers are fanatical about the size of their NC programs. It is also much easier to modify the G12/G13 canned cycle with Find and Replace on the control, so the operator can adjust the size of the hole. (If the operator were to just adjust the diameter offset for cutter comp, that adjustment would also affect other features being cut.)

 

It isn't something that I'm necessarily a proponent of, just mentioning another reason that some users prefer Circle Mill for cutting holes. (Personally, I'd rather just set my cutting parameters in the operation and be done...)

[guitar]

Some of my customers are fanatical about the size of their NC programs. It is also much easier to modify the G12/G13 canned cycle with Find and Replace on the control, so the operator can adjust the size of the hole. (If the operator were to just adjust the diameter offset for cutter comp, that adjustment would also affect other features being cut.)

 

It isn't something that I'm necessarily a proponent of, just mentioning another reason that some users prefer Circle Mill for cutting holes. (Personally, I'd rather just set my cutting parameters in the operation and be done...)

 Are those the same customers that do not understand drip feeding?

[Roger Peterson]

circlemill is great, helixbore is great, dynamic mill is great, and ramp contour is great.  Each of these have scenarios where they outshine the others, and a good programmer should know when to use each. 

 

The type of tool, does the tool centercut, the size of the tool relative to the finish size of hole, size of tool relative to pilot hole size, depth of hole relative to size of endmill, tolerances, tool life, programming time, run time, etc... all play a part in toolpath selection when doing a simple round hole or counterbore. 

 

For me circlemill is a toolpath I have always relied upon.  The ability to do multiple sizes in one toolpath, ability to plunge at center, the ability to specify a helix dia so the center of my tool is in pilot hole, the ability to do finish passes with a different speed and feed and cutter comp all in one toolpath, the roughing portion will outptu simple arc's for machines with limited memory, the ability to rough and finish with depth cuts, and here's a big one, copy a drill toolpath and convert to a circlemill (or use "last" selection during creation), etc... 

 

Circlemill is far from useless, but there are always scenarios where ramp contour, helix bore, or even dynamic mill and a separate finish toolpath are simply better.  Maybe a topic that discusses round hole applications and what worked best in specific scenarios would be useful.

 

JM2C

[Sticky]

 Are those the same customers that do not understand drip feeding?

 

Drip feeding sucks. If you can avoid it by using a canned cycle instead of a boatload of code why not?

[guitar]

Drip feeding sucks. If you can avoid it by using a canned cycle instead of a boatload of code why not?

 

It sounds like you are not using a good DNC software. Drip feeding is the way to go. 

[Sticky]

I use Cimco, it works fine for what I need, I can feed hold, restart the program wherever, etc. But I'm running an fms, and run lots of subs and macros, so dnc won't work. Even if it did, why would I want to inflate my program size? Aside from that, resident programs are more robust and reliable.

 

I only have 2meg memory on my machines so space has value.

[guitar]

Cimco can drip subs. Cimco rocks. 

[Richard Thomas - Mastercam UK]

 

 

Please shorten the wait time to auto select the center of an entity. 1 second is REALLY too long.

 

 

Guitar,

I was scanning through the posts looking for yours to reply to, I stopped when I saw all the CAPS   With regards to the one second delay when creating temporary midpoints, this sentence below is from the What's New X9 file.

 

"You can also hover and press [N] to avoid the one second delay."  I suspect this won't help you, but it might!

[guitar]

Guitar,

I was scanning through the posts looking for yours to reply to, I stopped when I saw all the CAPS   With regards to the one second delay when creating temporary midpoints, this sentence below is from the What's New X9 file.

 

"You can also hover and press [N] to avoid the one second delay."  I suspect this won't help you, but it might!

 

LOL. I was just hoping for 1/2 second. Unfortunately, I seldom have my fingers on the keyboard when chaining since one hand is on my trackball and the other on my space pilot pro. This is good info though. I might be able to assign a spacepilot button to the letter N. MUCH THANKS.

[Patternmaker706]

I had used X7 with no problems. Jumped X9, it works ok, a couple of things are quirky... It does crash occasionally. Surface high speed scallop works better in X7. X9 does not do vertical surfaces with that toolpath.

[Müřlıń®]

ok I found a reason to use circle mill...it is because of the other toolpaths that are in the same family.

You can copy paste and change tool type and get helix bore, drill and thread mill all in the same op....

[Guest]

It sounds like you are not using a good DNC software. Drip feeding is the way to go. 

 

Buying enough MEMORY is the way to go, NOT using outdated arcane technology.

 

[tim_h]

Not sure if this is an issue or something that I don't know how to turn on/off...

 

I just switched to X9 from X8.

When in X8 and I make a toolpath "active" (green check on toolpath folder) and  the wireframe geom that is used for that toolpath will highlight in yellow.

This doesn't happen in X9 and I can't find where I might be able to turn this handy little feature on...

 

This is different than the " only display associative geometry " function.

 

I followed jparis' suggestion on migrating X8 to X9 and it worked pretty darn good !

I just had to make changes to the existing config settings.

Perhaps the reason this is happening is that I missed something...

 

any thoughts ?

 

thanks !