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.
Code:
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.