[SBC Cycle]

Hello all,

I am just getting started with X9 after having it a few months now and I'm having a couple strange problems. First, I realize I should have proper training (and it's coming) but I believe this is probably a simple question to resolve.

I'm using X9 pretty much "out of the box" without messing with too many settings or configurations until I know what I'm doing but I believe I might have messed with some of these settings to fix my problem:



The problem is that when using the 3D toolpaths (in this instance OptiRough and Area Roughing) I can't seem to get my depths to "stick". For instance when trying to rough out the following part at a depth of 0.240" it always stops just short:

N52370 X-.2287 Y-.2933
N52380 Y-.3119
N52390 Y-.3177 Z-.2302 F21.4
N52400 X-.2284 Y-.3206 Z-.2304
N52410 X-.2275 Y-.3233 Z-.2306
N52420 X-.2261 Y-.3258 Z-.2308
N52430 X-.2229 Y-.3297 Z-.2311
N52440 X-.2192 Y-.3331 Z-.2315
N52450 X-.215 Y-.3359 Z-.2318
N52460 X-.2105 Y-.3381 Z-.2321
N52470 X-.2058 Y-.3396 Z-.2325
N52480 X-.2008 Y-.3405 Z-.2328
N52490 X-.1958 Y-.3406 Z-.2332
N52500 X-.1908 Y-.34 Z-.2335
N52510 X-.186 Y-.3387 Z-.2339
N52520 X-.1814 Y-.3368 Z-.2342
N52530 X-.1771 Y-.3342 Z-.2345
N52540 X-.1748 Y-.3324 Z-.2347
N52550 X-.1727 Y-.3305 Z-.2349
N52560 X-.1439 Y-.302 Z-.2377
N52570 X-.1397 Y-.2974 Z-.2381
N52580 X-.1359 Y-.2924 Z-.2385
N52590 X-.1325 Y-.2871 Z-.239
N52600 X-.1296 Y-.2816 Z-.2394
N52610 X-.1272 Y-.2758 Z-.2398   <----
N52620 X-.1236 Y-.2659
N52630 X-.1198 Y-.256

I also get the same when using Area Roughing, this time trying to finish the surface (0.250 DP):

N57020 G1 X4.4287 Y.3522
N57030 Z-.2105
N57040 G0 Z-.21
N57050 Z.1
N57060 X4.8599 Y-1.4131
N57070 Z-.2105
N57080 G1 Z-.2499 F30.   <----
N57090 X4.6971 Y-1.0819
N57100 G3 X4.693 Y-1.075 I-.0449 J-.0221
N57110 G2 X4.5089 Y-.4834 I.8109 J.5768 F13.4
N57120 X4.6929 Y.075 I.9966 J-.0189

I'm not sweating the few tenths of a thousandths. The real problem is when I try to use OptiRough or Area Rough with a "rest" operation. I always get a duplicate pass with a couple tenths difference and I believe the problem is related. It doesn't matter if I use "Previous Operations" or load up a "Stock Model" and use that. I always get a duplicate:

N1450 X4.6961 Y.075 I.994 J-.0189
N1460 G1 Z-.2244
N1470 G0 Z.0756
N1480 Z.1
N1490 X4.9977 Y-1.075
N1500 Z.0756
N1510 G1 Z-.2494 F30.   <----
N1520 G2 X4.9598 Y-1.0395 I.5026 J.575 F13.4
N1530 X4.7365 Y-.483 I.5404 J.5398
N1540 X4.9598 Y.0398 I.765 J-.0177
N1550 X4.9976 Y.075 I.545 J-.5468
N1560 G1 Z-.2244
N1570 G0 Z.0756
N1580 Z.1
N1590 X3.1024 Y-1.075
N1600 Z-.2244
N1610 G1 Z-.2499 F30.   <----
N1620 G2 X3.034 Y-.5016 I2.4153 J.5788 F13.4
N1630 X3.0905 Y.0251 I2.8127 J-.0353
N1640 G1 X2.9095

I could possibly load up a dummy file if anyone needs to look at my settings for the toolpath but if there is anything sticking out like a sore thumb and someone spots it could you please give me a bit of insight on what's going on? Here are the screenshots of the toolpath I'm talking about, first is OptiRoughing 0.240" DP and second is the finish pass 0.250" DP. Thanks guys and gals!

Attachment 316450 Attachment 316452

[Superman]

- you may be trying out Opt-rough & Rest-rough just to get experience. But that part could be done quicker using 2D operations
( ie pocket a zone between the 2 bosses, then 2D_Contour_Ramp the bosses )

What "Drive" features are you selecting for these operations ?
- any surfacing operations are best done selecting "minimal" features, the more items that are selected, the more complex it is to diagnose any fault
if you selected the whole solid, all flat faces will come into the equation
( try selecting just the walls. then add extra solid faces as needed )
- you could also use "Depths" to limit paths ( try setting absolute depths, not incremental )

But that being said, the 0.0001" error is less than half a bee's dick

Your programs seem long (5800 lines), check the "Tolerance" settings.....enable arcs in XY plane, & the tolerance slider to 50%
- Altering the Number sequencing is done in the Control Definition file.....open the Machine definition first then select the icon that looks like a screen....go to the "NC output" tab

[SBC Cycle]

Thanks for the reply Superman. You nailed it, I'm trying out the OptiRough & Area Roughing to get a feel for the 3D toolpath. Additionally, the part I am working on is a repeat job (an old one) and I have existing parts in stock that were programmed in BobCAD-CAM. I have found that when working with new software it is easiest to learn by starting with an old file that has already been done before with strategies that I am comfortable with - then finding the equivalent strategy in the new stuff. In this case I sort of needed the strategies to be the same because I have parts in stock and I want them to "look" the same visually on the finish cuts.

The toolpaths are remarkably similar but I'm not surprised as BCC and MC both use the Moduleworks engine under the hood for many of the 3D strategies. There are quite a few extra options/settings in MC (that are super sweet) to get used to. I'm not trying to force X9 to do what I want exactly but I'm looking for a similar workflow if possible.

Ok, now that you have a bit of background I can answer your questions (and thank you again for your input and experience)!

- I figured there was a similar 2D strategy to the OptiRough,, is Contour Ramp the one I'm looking for? I agree it would be quicker to use 2D and I'm working on getting used to creating the Levels and extracting geometry from the model. Almost all of the parts I make originate as SolidWorks files (I'm holding off using MC for SW just yet) so most of the 2D geometry I will work with will be pulled from the model. I'm struggling a bit with getting a handle on the differences between the WCS and the T/C Planes so sometimes when I create geometry from scratch it doesn't quite end up where I thought it would be but I'm getting better very quickly.

- Check surfaces are new to me entirely. I have gathered the idea behind the use for them and that should make my life a lot easier. You are correct that so far I am selecting the entire solid for the Drive surfaces. In the old software if I didn't it would mill right through some features unless I setup complicated boundaries (time consuming for the "real" 3D parts I work with). I got used to always selecting the entire part to minimize unintended consequences and time in programming.

- In BCC the Adaptive Roughing (same as OptiRough) and the Advanced Roughing (similar to Area Roughing) ALWAYS compare the model to the stock definition so the added benefit is eliminating air cutting almost entirely. I'm trying to pull off the same thing here which may not be necessary if I get a better handle on the 2D strategies. Again, for educational sake I'm trying to duplicate the same strategies I used in BCC in MC so my brain can make the connections. So far the only way I've found to optimize the toolpath is by using a "Stock Model" or "Use Previous Operations" and that's when the duplicate toolpath I'm getting pops up. I did find a thread here (you posted in that one as well) on how to do it differently but I didn't get it to work my first dozen tries. I found that boundaries will eliminate the air cutting pretty well but the time to create a good boundary is slower than just creating a 2D toolpath and associated geometry. More experience (and training) will fix that issue.

- I definitely used Depths - Absolute to limit the toolpath in the above example to only go to the first step (-0.250) and I think that might also be one of my sources of error. In the Steep/Shallow field when trying to get rid of the duplicate path using Rest material I entered Minumum Depth -0.250 and Maximum Depth -0.250. I recognize that I'm really bastardizing the use of this function but it doesn't matter what numbers I use, I always get 2 toolpaths at different depths. Is this to be expected when using "Rest Roughing"?

- The 0.0001" difference doesn't bother me at all, I was just wondering if it was related to the issue above when using Rest Roughing. I get 0.25 instead of 0.2499 if I use a different strategy (Finishing - Horizontal Area) and that works fine but the tool "marks" are different and it would look like someone else made these parts. I wondered if this was in an accuracy setting in the configuration screenshot I posted earlier.

- Lastly, I do get a lot of code but I've been hesitant to shorten it up using arc fitting. In both of the controls I use (Haas and Fadal) I've encountered various issues including but not limited to Arcs radius too large, arc radius too small, Arc sweep segment too short (this is the worst as it results in a "crop circle", usually breaking a tool). The controls don't seem to find the problem until they hit the offending line (graphics doesn't show it) and by then it is usually too late, I've gouged the part. I have plenty of machine memory available and I have the High Speed Machining option on the Haas so the extra code doesn't slow it down but I do want to investigate these settings in the future. You are very correct that this is just the smart thing to do but again, baby steps for now. On the sequence numbers I am using an increment of 10 for now in case I needed to hand edit the code. To my surprise I haven't need to do so at this point and I'm very pleased even if the post doesn't do everything exactly how I would want it. At a later date and after getting a copy of the Post manual from my VAR I want to edit the post to eliminate N sequence numbers altogether and only use them on the lines with the Tool change, also incremented by 10 so I can add probing routines at a later date.

Ok, I know that's a lot to read so I will summarize. Ignoring whether I'm using the "best" strategy for reasons explained above:

Is using Rest Roughing as a finish toolpath just a bad idea in general or am I not using it properly?
Is there an accuracy setting that will allow the OptiRough, OptiRest, Area Rough to go to the exact depth if it was necessary (blending purposes in general)?
Other than using "Stock Model" is there a better way to using the Rest Rough if "Previous Operations" is not available?

Thanks so much for replying and if no one wants to read all of this nonsense from a newb I completely understand. Your reply is very much appreciated and I will stick around to help other newbs when I feel comfortable doing so. This job is almost complete and they look just like the originals so I am very pleased!

[mkd]

Nice posts. Nice looking parts.
Filtering should not effect circles as it is related to point to point paths.

[Superman]

Nice posts. Nice looking parts.
Filtering should not effect circles as it is related to point to point paths.

???
If the toolpath ( on-screen display ) shows a circular move
...why would you want to have a point to point NC output, & end up with a arcs / circles made up of linear moves
( if you set the filter really badly, you could end up getting a hexagon ).


In effect , you are turning OFF the G2 / G3 functions on your machine

[SBC Cycle]

Nice posts. Nice looking parts.
Filtering should not effect circles as it is related to point to point paths.

Thanks! Not bad for used tooling start to finish, I thought I would have some bumps and bruises so I didn't sacrifice new tools. Mastercam performed like a champ.

I played with the tolerances tab screen and I think I follow what you mean here. I was able to reduce my code significantly by enabling simply enabling enabling "Line/Arc Filtering", unchecking the checkbox for Create Arcs In: G17 and changing the Line/Arc Tolerance from 0.00005 to 0.0005. An Opti-Rough toolpath on an arbitrary part when from 17,000 lines to 4,500. Is this what you meant by not effecting circles but the point to point path or should I be in the smoothing settings?

Pics attached are before and after

[SBC Cycle]

???
If the toolpath ( on-screen display ) shows a circular move
...why would you want to have a point to point NC output, & end up with a arcs / circles made up of linear moves
( if you set the filter really badly, you could end up getting a hexagon ).


In effect , you are turning OFF the G2 / G3 functions on your machine

Using the photos in the post above for reference, by unchecking the "Create Arcs In: " boxes (G17, G18, G19) am I leaving existing arcs unchanged while still filtering some point to point movements? My thought is that if it is an arc it will stay an arc and not turn into a slew of points (getting the "hexagon" effect). I did still get G02/G03 movements in the code and it looked like a whole lot less tiny linear movements.

Again, my worry is that by enabling Arc filtering I will get unusual arc segments. I do see the settings for Minimum/Maximum arc radius but that still has me worried about tiny chord length arcs in there. Thanks again for your reply :cheers:

[cadcam]

I have not read the hole post, But putting this out that the part that you cut using these paths really do not show the power of those paths. I would used the 2D HST paths toy really show how the software would excel on that path.

Like this path I did for a demo.
https://www.youtube.com/watch?v=YA8cCZ_u2Q4

[postwrtr]

Wow! Great looking parts.

I use optirough and 2D dynamic area more than any other tool paths because most everything I do is from barstock. The reason for the <truncated> values you are seeing in your paths is a combination of things. Any toolpath algorithm that uses a solid or surface as a part of its calculation will always have truncated values within the code if you see it or not it simply is a part of the math when calculating your path. The surface itself has a tolerance and the dialogue for the toolpath also has a tolerance and during calculation every point is compared against where the software thinks the solid body is or isn't using the aloud tolerances of the system and toolpath parameters to do so. It is sometimes very difficult to gather weather this is what you are seeing or not. The algorithm is always going to cut off or truncate these calculated points if the calculated point is in the exact same spot as the solid body or surface while taking into account the tolerance zone it is allowed to function in. You are looking for a depth value of exactly -.240 yet the output is several tenths off <-.2399> the toolpath algorithm is doing the right thing because the tolerance stack it is using to analyze the position on the model verse the position of the tool being used in the area there is an overlap therefore the depth must be cut back until it is outside the total tolerance zone therefore allowing the toolpath calculation to be on the right side of the material. When using a 2D toolpath this is not the case because this analyzing of surfaces is not performed a depth is given and should be seen in the code. Having said all of this I still use the 3D toolpaths as much as possible because I have to use stock model tracking to keep up with rest material. I will however beat the toolpath to death until I get the numbers I want to see or think I should. This is all a combination of your tolerances. There is an option for rest machining when using a stock model to ignore small cusps left over by previous tool paths used to produce the stock model this setting will remove the redundant passes you are seeing in rest machining.

I try to think of this in the same way a print relates to the physical part. You must have tolerances for each feature on a print and the part must lie within those tolerances. But it is easy upfront in a CAM system using a solid model that is perfect that the toolpath applied to that model would be perfect too but that is not the case. The math behind the calculation has to have some limited as to how many decimal places back should the calculations go? This is where the toolpath tolerances come into play allowing the programmer to apply as a variable within the calculation the accuracy of the math being done to achieve a toolpath that will provide the desired results and not waiting 4 hours to calculate a more perfect path. I would think with some investigation into the system tolerance of the solid model you are machining against and the cut tolerance you will be able to achieve the correct numbers in depth you are looking for. Just keep at it while considering these tolerance overlapping possibilities.

one more thing to consider is that 3D tool paths look too at the corner radius of the tool and the corner radii on the model if you are machining vertical walls that have a floor corner fillet larger than the tool corner then the tool must cut at a higher level in Z so as to not violate the corner of the model the roughing tool path will do just that and not take another z depth of cut to achieve proper depth while laying off of the wall in order to preserve the corner radius fillet

So many possibilities here for your outcome but there is something set that is protecting the path from gouging the model. Having started programing 5 axis machines 20 years ago with notepad and a calculator I always want my code to be neat and exact. It has helped me through the years to not only look at the output in numbers but look long and hard at the toolpath on the screen rotating the model over and over as if to walk behind the path of the tool taking time to understand how the algorithm is arriving at its result.

Parts look great though