For those of your that find issues with the V25 software please report them.
Use this link to report any issues you find with the New V25
Report | BobCAD-CAM
Thank you
For those of your that find issues with the V25 software please report them.
Use this link to report any issues you find with the New V25
Report | BobCAD-CAM
Thank you
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
I opened up the 3D example and applied the advanced roughing toolpath.
The function: CAM Part/milling tools/compute all toolpath does nothing
When I post the code it seems incomplete.
I can't save or load features
This is the same for me on two different machines.
yes please report these issues!
We need to re create the steps so attached a file and walk through the steps you took 1 by 1 .
This will help us fix any issues that you guys come up with.
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
.
Bump ! !
:rainfro::rainfro::rainfro:
.
https://dl-web.dropbox.com/get/Publi...swf?w=73881f97
Here is a screen cast documenting my problems with V25. let me know if you have trouble viewing.
Compute all toolpath doesn't work for me.
Save/Load feature is greyed out.
Posted NC data is incomplete
Steven
In demo mode, the compute all and save/load are disabled by design, so it's working the way it's designed to. In order to unlock those options you need a licensed version.
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
.
Al
Still not able to seperate chamfering from a Feature in V25 so that all chamfers in a program can be done in a single tool change, currently have to make a number of Chamfering Features to be able to achieve this.
Also again on chamfering can we be able to choose the same Chamfer tool eg Chamfer Mill for all chamfering, currently the software only throws up a "Chamfer Tool" for chamfering drilled holes and a "Chamfer Mill" for profile/pocket chamfers, currently means having to have 2 tools in the machine when one would do and extra tool changes
Any idea if this will be in a V25 update anytime soon ? ? ?
Regards
Rob
:rainfro::rainfro::rainfro:
.
"Also again on chamfering can we be able to choose the same Chamfer tool eg Chamfer Mill for all chamfering, currently the software only throws up a "Chamfer Tool" for chamfering drilled holes and a "Chamfer Mill" for profile/pocket chamfers, currently means having to have 2 tools in the machine when one would do and extra tool changes "
Could a guy change tool number in preditor editor so they were both the same?
Well you could change the tool number in the crib to be the same for the chamfer tool and mill so that they are the same.
Also when you post you have the option to post by tool, What this does will post all the ops for that tool in the tree. Is this not working?
Al
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
If you post by tool the software will look through the job tree and post all features that have the 1 tool, then 2nd etc.
It seems to work just fine on my end, am I missing something?
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
Introduction
The Machine Order dialog box allows you to specify how the tool changes in the program are optimized. The machining order can be optimized by Individual Feature, Individual Tool Per Machine Setup or Individual Tool.
Navigation
To access the Machining Order dialog box, do one of the following:
In the CAM Tree, right-click Milling Tools, click Default, and Machining Order. Any changes made here affect all new parts created thereafter.
In the CAM Tree, right-click Milling Tools, click Part, and Machining Order. Any changes made here only affect the current part.
The Machining Order Parameters
View the Machining Order dialog box
In order to fully understand the Machining Order, there are some terms that must be clarified. All milling features are inserted in the CAM tree, in a Machine Setup. The Machine Setup defines the machining origin for all features contained in the Machine Setup. Any part can have multiple Machine Setups with multiple features in each. Each milling feature is used to define and create toolpaths for a specific purpose, such as a Hole feature. The feature is executed using one or more operations. For example, a Hole feature is composed of a Center Drill operation, a Drill operation, and an optional Chamfer operation. In conclusion, a part can have multiple Machine Setups, which can contain one or more features, which contain one or more operations.
Individual Tool
When selecting Individual Tool, the Machining Order is optimized by completing all possible operations with each tool before changing the tool and moving on to the next operation. This is done across all features to reduce the number of tool changes. This method is useful, for example, when drilling operations of different sizes are performed with multiple drilling features. All center drill holes are drilled before changing the tool. Then all drill holes of the same size are drilled before the next tool change. This process is repeated until all features are completed.
Individual Feature
When selecting Individual Feature, all operations are executed for each feature before moving on to the next feature. This method does complete all possible operations with each tool before making a tool change as in Individual Tool, but it does not complete similar operations with the same tool across multiple features. This method is useful when one feature operation must remove stock material before the next feature operation can start.
Individual Tool Per Machine Setup
When selecting Individual Tool Per Machine Setup, the Machining Order is optimized in a manner similar to Individual Tool. The difference is that each possible operation for each tool is executed, before a tool change, across all features contained in a Machine Setup group. This method is useful when using a different Machine Setup for each side of a part.
Example
In this example, two Tap features are inserted in the CAM tree. Even though each Tap feature is a different size, the center drill and chamfer tools used for each are the same size. The operations of each feature are shown next:
Features
Tap Feature 1 Operations:
Center Drill 1
Drill 1
Chamfer 1
Tap 1
Tap Feature 2 Operations:
Center Drill 2
Drill 2
Chamfer 2
Tap 2
Individual Feature
The order of operations when using Individual Feature:
Center Drill 1
Drill 1
Chamfer 1
Tap 1
Center Drill 2
Drill 2
Chamfer 2
Tap 2
Notice that the order is the same as the Tap Feature 1 and Tap Feature 2 operations combined.
Individual Tool
The order of operations when using Individual Tool:
Center Drill 1 and 2
Drill 1
Chamfer 1
Tap 1
Drill 2
Chamfer 2
Tap 2
You can see that for Individual Tool, the Center Drill operations for each feature are executed together. Notice in step 3 that even though the chamfer tool is the same size for each feature, both chamfers can't be executed at the same time because Drill 2 has not yet been executed. The reason that both Drill operations are not completed before the Chamfer operations is that the original order of operations, shown in Tap Feature 1 and Tap Feature 2, is still followed.
Individual Tool Per Machine Setup
The following lists show the same Tap Feature 1 and Tap Feature 2 in one Machine Setup, and then Tap Feature 3 is added in a separate Machine Setup.
Machine Setup 1
Tap Feature 1 Operations:
Center Drill 1
Drill 1
Chamfer 1
Tap 1
Tap Feature 2 Operations:
Center Drill 2
Drill 2
Chamfer 2
Tap 2
Machine Setup 2
Tap Feature 3 Operations:
Center Drill 3
Drill 3
Chamfer 3
Tap 3
The order of operation for Individual Tool Per Machine Setup:
Center Drill 1 and 2
Drill 1
Chamfer 1
Tap 1
Drill 2
Chamfer 2
Tap 2
Center Drill 3
Drill 3
Chamfer 3
Tap 3
Notice that the order of operations is optimized like Individual Tool, within each Machine Setup. The operations of one Machine Setup are completed before moving on to the next Machine Setup.
--------------------------------------------------------------------------------
TIP: The order of operations that can be edited are defined in the Tool Pattern Global and Tool Pattern Program dialog boxes.
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
Al
As the heading says, your examples are valid but you are using all the same type of feature ie drilling with/without tapping, yes that will bring up the same tool for the chamfer so in your examples using the "tool dominant" selection will work fine, the problems start when we start mixing up different types of features with some at different Z positions.
See the attached file, it is a very very simple everyday job with a piece of stock with 3 holes all the same diameter, 2 on the top of stock and 1 in the small pocket.
Job is :-
Mill small oval pocket
Drill 3 3.35mm holes
Chamfer holes, pocket and outer shape
If I want to have only a single tool change per tool then this simple job appears to require no less than 7 seperate features.
Some of this can of course be simplified by saving out features for drilling, chamfering etc, etc and then just loading and editing but unless I am getting very senile in my old age then I don`t see any other way to do it.
I have tried changing the "assigned tool" and the tool will change from the "chamfer tool" as used on the drilling to the "chamfer mill" as used on the other features but although the tool designated changes the tool number doesn`t.
Please don`t misunderstand this, the software does work OK, V25 is excellent, it`s not that the job can`t be done this is all just "Wish List" stuff
Regards
Rob
:rainfro::rainfro::rainfro:
.
Hey Al, I noticed when I made a bug report last week that under the dropdown menu for "Version" it doesn't list V25 yet.
I can't seem to get a helical entry on the 2 AXIS - Thread feature.
I have selected "Through" hole (blind hole I don't think allows helical entry) but the Z move is generated after the compensation move not with the actual lead into the cut.
This was fixedCode:(NEXT CUT - NEXT TOOL) (JOB 8 THREAD MILLING) (FEATURE THREAD) (TOOL #10THREAD MILL) N109 T10 M06 N110 G90 G54 X0. Y0. S397 M03 N111 G43 H10 D10 Z0.1 M08 N112 G00 Z2. N113 Z0.1 N114 G01 Z-0.4348 F0.5562 N115 X0.2236 Y-0.3 F1.1123 N116 Z-0.42 N117 G17 G03 X0.5236 Y0. I0. J0.3 N118 X0.5236 Y0. Z-0.3019 I-0.5236 J0. N119 G01 Z-0.2871 N120 G03 X0.2236 Y0.3 I-0.3 J0. N121 G01 X0. Y0. N122 G00 Z2. N123 M05 N124 G91 G28 Z0. N125 G91 G28 Y0. N126 T9 M06 N127 M02
Even worse, it moves in Z while the thread mill is still engaged. This feature needs a lot of work.
I was able to duplicate your issue by setting the lead radius wrongly, if the radius is set to a value less than the radius of the tool then it will be clear of the material during any of the lead-in/out moves so it shouldn`t be a problem.
It seems to work OK here using "Blind" hole and "Helical" entry as long as the lead radius is less than the tool radius of 9.5mm for the 19mm tool in your example
Sorry, that`s all I have
BTW That goes for cutting "bottom up" as well as "top down"
Regards
I played with the radius value all the way from 0.01 to full radius of the thread and I still get both Z moves in the wrong spot, not with the arc in/out.
My thread is an internal M45 x 3mm.
Here are the parameters I used at the machine:
Diameter = 0.748
Pattern = Bottom Up
Thread Type = Inside
"Through"
Right Hand
Thread Diameter = 1.7972
Thread Height = 0.1023
Thread Pitch = 0.1181
Thread PR = 8
Depth = 0.420
Helical Lead In/Out = 0.2623
The code from BobCAD:
If I move the Z on line 148 to line 149 and the Z on 151 to 152 it makes a perfect thread. As it is posted, at line 150 the thread has finished one complete pass but is still parked inside the thread. The next move the tool goes straight up. Then it exits the thread.Code:(NEXT CUT - NEXT TOOL) (JOB 9 THREAD MILLING) (THREAD-M45X3) (TOOL #10THREAD MILL) N141 T10 M06 N142 G90 G54 X0. Y0. S398 M03 N143 G43 H10 D10 Z0.1 M08 N144 G00 Z2. N145 Z0.1 N146 G01 Z-0.4348 F0.5576 N147 X0.2623 Y-0.2623 F1.1152 N148 Z-0.42 N149 G17 G03 X0.5246 Y0. I0. J0.2623 N150 X0.5246 Y0. Z-0.3019 I-0.5246 J0. N151 G01 Z-0.2871 N152 G03 X0.2623 Y0.2623 I-0.2623 J0. N153 G01 X0. Y0. N154 G00 Z2. N155 M05 N156 G91 G28 Z0. N157 M01
What am I doing wrong if you don't mind Rob? I moved that lead in radius up and down and I couldn't get rid of it.
Here is the code for my set up for a 3mm pitch in a 45mm dia thread using 1 pitch per revolution going "top down" which outputs as a single point thread mill doing 5 revolutions for a 15mm depth in the V25 simulation.
(JOB 2 THREAD MILLING)
(FEATURE THREAD)
N2981 T02 M06
N2991 S97 M03
N3001 G90 G54 X0. Y0.
N3011 G43 H02 Z1. M08
N3021 G01 Z.375 F3.5733
N3031 X3.5 Y9.5 F7.1466
N3041 Z0.
N3051 G17 G02 X13. Y0. I0. J-9.5
N3061 X13. Y0. Z-3. I-13. J0.
N3071 X13. Y0. Z-6. I-13. J0.
N3081 X13. Y0. Z-9. I-13. J0.
N3091 X13. Y0. Z-12. I-13. J0.
N3101 X13. Y0. Z-15. I-13. J0.
N3111 X3.5 Y-9.5 I-9.5 J0.
N3121 G01 X0. Y0.
N3131 G00 Z1.
N3141 M05
N3151 G91 G28 Z0.N3161 G91 G28 X0. Y0.
N3171 T01 M06
(END OF PROGRAM)
N3181 M30
%
Second code is the same sizes but now going from "bottom up" using 5 threads per revolution which outputs as a multi point (5 or more) thread mill doing 1 revolution for the same 15mm depth in the V25 simulation.
(JOB 2 THREAD MILLING)
(FEATURE THREAD)
N2981 T02 M06
N2991 S97 M03
N3001 G90 G54 X0. Y0.
N3011 G43 H02 Z1. M08
N3021 G01 Z-15. F3.5733
N3031 X3.5 Y-9.5 F7.1466
N3041 G17 G03 X13. Y0. I0. J9.5
N3051 X13. Y0. Z-12. I-13. J0.
N3061 X3.5 Y9.5 I-9.5 J0.
N3071 G01 X0. Y0.
N3081 G00 Z1.
N3091 M05
N3101 G91 G28 Z0.
N3111 G91 G28 X0. Y0.
N3121 T01 M06
(END OF PROGRAM)
N3131 M30
Obviously I haven`t run these at a machine, it`s 1.00am here and I`m at home but the code looks "clean" to me
Attached are the files, you will notice that I have set the lead in and lead out differently, Helical in and Circular out and the lead radius is set to the radius of the tool, 9.5mm.
It all seems to be OK here, I have also run these two sets of code through my Predator backplot and again I can see no problems of "gouging" Z moves while in the material.
If they are there then I`m not seeing them, could maybe my age and the time of 1.15am :tired: :tired: :tired:
Hope it helps and I hope I got all the colours right for easy reading
The Leads are in Green and the thread cuts in Blue, I think
Regards
LOL, I hope you are in bed finally! In your second example file (19mm Thread Mill Test-2.bbcd) the helical lead in is not being posted. I expect that as the help file says that the helical lead will not work with a blind hole (on departure but it seems to not work on entry either).
However, if I change the hole to a "through" hole in that file, it posts the odd Z move. I did the update also. It's still there.