[RAF.]

Is anybody having problems Advanced Rough/Adaptive Rough In V25 Pro, Yes I know it is a stupid looking tool path but that is what Bobcad is putting out. Is it still that intermediate step thing that is still giving trouble? If it is would be nice to have it fixed.
Maybe some one can try this and see if they can get it to work without gouging.

V25 Build 966

[RAF.]

Al
Is this tool path strategy suppose to gouge like this or is it broken?

[aldepoalo]

I haven looked at your file but what is the problem the way you see it?

[jrmach]

Here is what I get with my simulation and with preditor back plot.I do not show what you do.Or is that a pic of the part,in the middle of a cut ?

[dertsap]

if your cutting aluminum , I'd suggest un-checking the adaptive rough and click on zigzag . Otherwise you've got an incredible time waster with your current setting

[RAF.]

I'm thinking that I should be able to use Advanced Rough/Adaptive Rough on this solid but I am getting a rapid down at these points. and my cutter will probably not like it very much. Nor will the part

[RAF.]

Here is what I get with my simulation and with preditor back plot.I do not show what you do.Or is that a pic of the part,in the middle of a cut ?

Thanks Jr for looking at that The picture with the red marks is rapid downs a step thru at line move 30531 should show up at least it does on my sim. I am going to step thru Predator backplot at that area and see what I can find.

Also thanks dertsap for your help and thoughts but I am trying to find out what is wrong with this tool path strat.

Yea never know maybe this could be a Government Job where time and money is not a problem

[jrmach]

Your rapid is set to 29 ipm,would not be a problem in my machine in aluminum.Adjust it down if you are running a small machine.It is only going rapiding down a little ways.

The rapid should be what is set in plunge feed? ? ?Not the rapid of the machine itself ? ? ? ? ?

[RAF.]

Here are some more pics of what is happening. It is like it puts out Z code in reverse at the bad spots. You can run it and it will look fine, but if you run a crash report it will show problems and then run slow thru move list you can see what it is doing. It looks like it picks up at plunge feed speed and then rapids up and over and down all the way a rapid.
Yes we can have work-arounds and slow our rapids down if working with hard materials but wouldn't it be better to have the program work properly.
I have got it to put out a good Tool path buy increasing cutting depths and also increasing the intermediate steps which doesn't make much sense to me.
And again yes It is a stupid looking tool path but its V25 PRO Advanced Rough/Adaptive Rough so there must be some reasoning for it.
I would really like to get this tool path working correctly, hopefully there is an easy fix or is it operator error?

[aldepoalo]

Ok, I am at the office now and have a chance to look at your file.

1) I am not sure what you mean by stupid looking tool path. The adaptive roughing tool path option is a high speed style tool path. You would see a similar tool path generated with dynamic milling from Mastercam, or I machining from Solidcam or profit milling from Esprit.... The list goes on an on, and over the last few years this style tool path is or has become the preferred method for material removal.

To better understand some of the concept of high speed machining check out this link, it will help you understand why the tool path looks the way it does.

High Speed Machining (HSM) for CNC Milling


2) When I simulate your part the way you have it setup I do see the red plunge moves indicating the tool rapid down to depth.

Attachment 203788

Not knowing what machine or what material you are running, I will reserve any comments about if this is the right approach to make this part with your equipment and focus on getting good results some little changes to your settings.


Here are your settings for Rapid Movements:

Attachment 203790

You'll notice you have the same value set for all 3 options of .1 - I find it a good practice to use different values for for these. The first thing I would change is your clearance plane to .5 you rapid plane to .25 and keep your feed plane at.1

You may notice your clearance plane is grayed out, you'll have to edit your machine setup to change this value. You can edit the rapid and feed plane at the feature level.

Attachment 203792

I would say this is not a must have, but I would say it's a good practice....

Making these changes alone will not effect the rapid to depth issues you that you are having.

N11264 G01 Z-0.8375
N11265 G00 Z0.25
N11266 X0.5001 Y0.8351
N11267 Z-1.25 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N11268 G03 X0.4142 Y0.82 I-0.035 J-0.0532 F59.5061
N11269 X0.4054 Y0.7912 I0.0309 J-0.0253
N11270 G01 X0.4066 Y0.7749
N11271 X0.4146 Y0.755
N11272 X0.4309 Y0.727
N11273 X0.4437 Y0.7084
N11274 G03 X0.4559 Y0.6954 I0.0276 J0.0137
N11275 G02 X0.5654 Y0.6098 I-0.4319 J-0.6653
N11276 X0.7137 Y0.4274 I-0.5868 J-0.6284
N11277 G03 X0.7321 Y0.4123 I0.0396 J0.0295
N11278 G01 X0.744 Y0.4084
N11279 X0.792 Y0.4053
N11280 X0.7994 Y0.4054 Z-1.2499
N11281 X0.8067 Y0.4068 Z-1.2496
N11282 X0.8135 Y0.4095 Z-1.2493
N11283 X0.8198 Y0.4135 Z-1.2489
N11284 X0.8252 Y0.4184 Z-1.2472
N11285 X0.8293 Y0.424 Z-1.2444
N11286 X0.8322 Y0.4298 Z-1.2385
N11287 X0.8344 Y0.4369 Z-1.2336
N11288 X0.8351 Y0.4438 Z-1.232
N11289 X0.8346 Y0.4508 Z-1.2312
N11290 X0.8323 Y0.459 Z-1.2308
N11291 X0.8283 Y0.4666 Z-1.2305
N11292 X0.8228 Y0.4731 Z-1.2303
N11293 X0.4731 Y0.803
N11294 X0.4644 Y0.809 Z-1.2306
N11295 X0.4546 Y0.8127 Z-1.231
N11296 X0.4475 Y0.8136 Z-1.2314
N11297 X0.4405 Y0.8133 Z-1.2331
N11298 X0.4342 Y0.8118 Z-1.2361
N11299 X0.4283 Y0.8094 Z-1.2417
N11300 X0.4224 Y0.8057 Z-1.2466
N11301 X0.4175 Y0.8013 Z-1.2483
N11302 X0.4134 Y0.7961 Z-1.2491
N11303 X0.4095 Y0.7889 Z-1.2495
N11304 X0.4073 Y0.781 Z-1.2498
N11305 X0.4068 Y0.7729 Z-1.25
N11306 X0.4081 Y0.7456
N11307 X0.4096 Y0.7391
N11308 X0.4154 Y0.7265
N11309 G03 X0.428 Y0.7132 I0.0381 J0.0236
N11310 G01 X0.4551 Y0.696
N11311 G03 X0.4847 Y0.6907 I0.0214 J0.0337
N11312 X0.5593 Y0.7964 I-0.0151 J0.0898
N11313 G01 Z-0.9625
N11314 G00 Z0.25
N11315 X-0.8349 Y0.5002
N11316 Z-1.25 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N11317 G03 X-0.8197 Y0.4143 I0.0537 J-0.0347 F59.5061

These are the block of code that I get when that are showing the rapid down to z which is a problem. It's nice to know the simulate is picking up the problem.

Ok so the next thing that I would look at is your machining tolerance.

Here is what you have the software set to:

Attachment 203794

When roughing a part out I would loosen this tolerance up. More likely I would have this set to .001. Adjusting this alone will not remove your rapid issue, but again it's good practice Having your roughing tolerance set to .0005 is way more accurate then it needs to be, and it also will result in longer computing time unnecessarily. Un less there is a reason to rough at this tolerance ( which I can't think of ) I would reduce this value to .001

Making the above 2 changes had no effect on the rapid issue. So from here are have 2 choices, either change the style of tool path I am use, or adjust additional settings. Depending on the geometry you are working with, there can be geometric conditions that cause "problems" with the tool path algorithm. You would want all tool path to be 100% bullet proof, but the reality is, they aren't. No CAM systems are and any vender that tells you so, is well selling you... So when you are getting results that aren't optimal, changes your settings or change your approach.


After playing around with some of the tool path settings like:

Depth of cut
Leads
# of intermediate steps ( or setup up in other CAM systems )

I found that the number of intermediate is what was causing the issue.

When set to 2 = rapid issue
When set to 1 = no rapid issue
When set to 3 = rapid issue
When set to 4 = rapid issue

So my choices are either to use a value of 1 for intermediate step or to set to 0 and use a Z level finish to re rough the step downs if I want to use this style of tool path.


So now we know where the problem is coming from and what steps to take to eliminate the issue. You other option would be to change the style of tool path you are using. By removing adaptive roughing

Attachment 203814

You'll be using a more traditional offset type tool path and making this change alone with the file settings you used eliminates the issue. This will remove the air cutting you are seeing in the adaptive roughing as the tool repositions back for the next cut. . Using zig cut pattern keeps the tool in the cut and is more likely the type of tool path you are expecting.

**** Warning ******

To eliminate dog leg rapid potential issues make sure to use the following option:

Attachment 203816


**** Warning ******


I am not sure if this is the answer you were looking for, but it should out line the steps and work flow I followed to evaluate your part and get the chips flying. To be fair when within 2 mins of opening you file I had a solution.

[RAF.]

Al
Thanks for the help with the tool path. To call the tool path stupid is maybe much but it has been described in the past as similar.
I do relies that this is a HSM and that they do look different.

Al can you tell me how or what you are using the find the # of Gcode line where the bad Z rapid is?. It is so easy to edit that Z rapid to a Z feed move beings there tis only 3 in this file.

Thanks again
RAF

[aldepoalo]

I used the predator editor ( Pro ) ran a back plot / simulation knowing where the problem was I just looked for it in the sim then in the code. The other option would be to look for G00 moves, but that's hard to do not having the sim.... If you don't have the predator editor upgrade as I like to call it, you should pick up a copy. If you don't want to use the predator editor there are other back plotter / simulation programs for you to choose from.

And yes the problem is we are getting rapid to depth in 2 or 3 sections where we shouldn't be. You could easily find these blocks and just add a G01 in front of the Z and a F at the end to have it feed to these spots eliminating the problem.

As far as why there is a rapid in the first place, there seems to be a sorting issue going on in the back round. These moves are coming from the intermediate cuts, which should be posted bottom up after the part has been roughed out. For some reason when set to 2 or move intermediate cuts on your file, there are being posted out of order....

Again not knowing what machine and material I still would recommend using the standard zig option instead of the adaptive roughing. It does a great job and my guess would run better on your machine...

When dealing with HSM there are chip thinning concepts for feeds and speed that need to be applied. Also a typical depth of cut would be the same at the diameter of the tool with a step over of 10% that diameter.

I hope this information has help you get going and answered you questions about this topic. If there is anything else I can help with please let me know.

[bobcad guy]

The problem is adaptive ruff, it has a rapid issue that was reported long ago, that probably lingers on right into version 26. Justdont use adaptive ruff, or, the old workaround, hand fix what the cam program is supposed to output

[dwood]

RAF

if you select by level under processing, recompute ,seems to fix your issue
i also would use a lead in

dw

[RAF.]

RAF

if you select by level under processing, recompute ,seems to fix your issue
i also would use a lead in

dw

dwood
Ran the file with only changing in the Options / Area to Level and ---wala---no feed/rapid showed up in the report

Thanks for the help Hope it will work on some other paths also

[aldepoalo]

I write a book, D Wood writes a sentence... lol

Attachment 203988

I knew it had to do with a sorting I should have found that one! Great job D wood!