[Ben S]

I am using V24. A pocket I programmed is coming out .005" to .010" too small. I left Side Allowance as zero so it should not leave anything for a finish pass right? I ran the program twice to make sure it wasn't just tool deflection but it is still too small. The cam file and post are attached. Thanks for your assistance.

Ben

[Ben S]

I don't see a way to include a G41 wear offset in the program either. The check box called Machine Compensation seems to only apply to the finish pass but even when I turn that on I don't see it in the code. I ended up just changing the diameter of the tool in the tool library. Is this the way people normally do this?

This seems like something that would have already been covered but I didn't find anything in my search.

Ben

[jrmach]

Dimension your pocket to make sure you drew the size you wanted.Other than that,it would be a problem with probably tooling..005 too small is only .0025 a side.I have bought end mills off E-Bay that are that undersized and more.
Also,what material you cutting?
Also,don't run the program twice,just leave a little for a finishing pass.You can use same tool as roughing.

[Ben S]

Good point, I'll mic the tool. It's not brand new so I guess it could be real wear. Material is aluminum. When programming a finish pass is there a way to get it to cut the finish pass at each depth? My pocket is deeper than my flute length.

[Ben S]

Tool measures .248" on my .0005" Mitutoyo mics so I guess that could account for most of the problem. I'll keep a close eye on it the next time I'm using a new tool. Would still like to know how to cut a finish pass at each roughing depth and how to use the Machine Compensation feature correctly so I can put in a wear offset at the control.

[RAF.]

Ben
If you use a worn tool won't you get a step in your pocket and have other problems if deeper than flute?

[The Engine Guy]

Tool measures .248" on my .0005" Mitutoyo mics so I guess that could account for most of the problem. I'll keep a close eye on it the next time I'm using a new tool. Would still like to know how to cut a finish pass at each roughing depth and how to use the Machine Compensation feature correctly so I can put in a wear offset at the control.

To be able to post G41/G42 tool diameter offsets to be called at the machine you need to check your Post Processor has the "cc" (Cutter Compensation) active, remember it is only active on your finish cuts

Open your Post in Notepad and for starters look for the blocks 2,3 and 4, don`t know what post you are using but it should look something along the lines of the extract below :-

n,absolute_coord,cancel_drill_cycle,"G40",inch_mod e,"G17"
" "
n,rapid_move,incremental_coord,"G28","Z0."
n,rapid_move,incremental_coord,"G28","X0.","Y0."
" "
system_comment
feature_name_comment
comment_start"TOOL #",list_tool_number, "-",(tool_label),comment_end
n,t,"M06"
n,"M00"
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,
n,rapid_move,length_offset,coolant_on
output_rotary_angle
n,cc,

3. Tool change
n,"G40"
n,coolant_off
n,spindle_off
n,rapid_move,incremental_coord,"G28","Z0."
n,"M00"
" "
system_comment
feature_name_comment
pass_name_comment
comment_start,"TOOL #",list_tool_number, "-",(tool_label),comment_end
n_forced,t,"M06"
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,
n,rapid_move,length_offset,coolant_on
output_rotary_angle
n,cc,

4. Null tool change
" "
system_comment
feature_name_comment
" "
n,s
n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angl e,
output_rotary_angle
n,cc,

If the lines in Red are not there then put them in where you want the G41D** line to appear in your code.
Here is some code as generated by the post shown above :-

( TOOL #2 - 12.700 Dia. 0.000 CRad. 4 Fl.38.100 CL)
N39 T02 M06
N40 S1879 M03
N41 G90 G54 X-28.638 Y34.714
N42 G43 H02 Z2.54 M08
N43 G41 D02
N44 G01 Z-3. F381.8741


Note that the Tool diameter offset is directly after the Tool height offset in this example.
If your machine control won`t do both an H1 and D1 offset (Some controls won`t do it like Fanuc 0M) the you should be able to use a different offset number, for example if you have total 100 tool offsets then they can often be split into say 1~50 for Height off sets and 51~100 for diameter offsets, if that were the case then go to line 267 in your Post and change the "0" to "50" and the Post will then add 50 to the D numbers so you would then have something like:-

267. Amount to add to tool # for tool register value? 0

G43H01
G41D51

Hope that is of some help to you.

Regarding the Finish at every depth I think you will have to do the feature to the peck depth you want and then save the feature out and re-load it and just change the depth on each new feature, still don`t see how you can do it at all if your tool flute length is too short but I am probably just missing something obvious, maybe you have tools that have smaller shank than flute ? ?

Regards
Rob
:rainfro: :rainfro: :rainfro:

[Ben S]

Engine Guy, thank you for the detailed response. I will have to take some time to go over the post and see if it includes the lines you highlighted. I'm not experienced at reading posts so that will take time. It is a default post that came with the software, though, so I would think it would be set up to work with the features in the software, right?

As to my finish pass question, I use tools that have the same cutting diameter and shank diameter. If my feature is deeper than the flute length I cut several roughing depths. If it cuts only one finish pass at full depth then the shank will interfere with the wall above. But if it cuts a finish pass at each depth then there is no problem. Make sense? In Mastercam there is a check box for this. I'm not seeing a way to do it in Bobcad.

Thanks for the input.

[mmoe]

Engine Guy, thank you for the detailed response. I will have to take some time to go over the post and see if it includes the lines you highlighted. I'm not experienced at reading posts so that will take time. It is a default post that came with the software, though, so I would think it would be set up to work with the features in the software, right?

As to my finish pass question, I use tools that have the same cutting diameter and shank diameter. If my feature is deeper than the flute length I cut several roughing depths. If it cuts only one finish pass at full depth then the shank will interfere with the wall above. But if it cuts a finish pass at each depth then there is no problem. Make sense? In Mastercam there is a check box for this. I'm not seeing a way to do it in Bobcad.

Thanks for the input.

There isn't the option to do this automatically within a pocketing feature or profile feature. You can do it in two steps though, and you have to sort of trick Bobcad into doing so. I also use V24, so this should be pretty much exactly the same for you.

For a pocketing feature:
First, go to your cam tree and right click on "Milling Tools", then select "Part-->Tool Pattern". This will bring up the lists where you can select how each feature will operate. You then click on Pocket which will display the operation lists. To the left you will see "With Chamfer" and to the right you will see "No Chamfer". You can highlight any operation and delete it with the "Delete" button below that list. Personally, I rarely need to chamfer anything, so I've set up the "With Chamfer" side to have only the "Endmill Rough" operation while I've left the "No Chamfer" side alone in case I want the option of a full height finish pass. You could also set up the "No Chamfer" side to only have "Endmill Rough" if that's more convenient for you. From now on, you can produce a roughing only pocket routine. If you want the change permanent, you'd have to go the "Milling Tools-->Default-->Tool Patterns", but I'd suggests saving the default tool patterns to a backup file first in case you wish to restore the factory settings.

Next, start a CAM window for 2d pocketing, select the geometry and then either check or don't check the "Chamfer" box depending on how you set up the above so that you have a roughing only feature. Now, you can set up the operation as normal for the tool, then in the "Patterns" window check "No Profile" along with any other preferences here. In the next window, "Parameters", set the side allowance to whatever you want to remove with your finishing pass and the bottom allowance to "0". Check "Multiple Steps" and set them to your preferences, then do the rest of the windows as normal until you click "Finish". This will produce a pocket without a finish pass, but also with an allowance on the sidewall which can be cleaned up with a profile pass. Actually, to be more correct, it will still produce a finish pass that will cut air, but it will be located within the pocket you already roughed out, so there will still be material to cut for a finish pass (not sure why it still insists on generating that profile pass, but it does). Now you would start up a CAM feature with 2d Profile, and make sure you do the roughing pass with NO ALLOWANCE. This will allow you to do multiple steps down as if it's a finish pass and the profile feature will automatically skip the finish pass that it would normally do if you set an allowance.

If it's a profile pass, you can go into "Milling Tools-->Part-->Tool Pattern" again and set the "Contour" feature to have only a "Endmill Rough" pass. At this point, you now have to do two different features. One with an allowance, then the next with no allowance. You can set them both to have multiple passes as needed.

All that said, and without seeing the parts you're working with, it may also be a good idea to add another piece of software too your computing toolbox. I've started using EstlCAM 2.5d, which costs $25 (no joke), to produce some of these toolpaths that don't fit into the standard Bobcad workflow. Bobcad offers more overall and it's price reflects this, but when it comes to 2.5d work off of simple 2d DXF drawings, EstlCAM is a great addition to fill in the gaps. In the tool setup for EstlCAM, you can define the maximum cutting depth per pass for each tool, which means that as you generate tool paths it will automatically take the max depth into account and you don't have to do anything special. You also define things like the amount of overlap, which it will then apply as specified for each tool automatically as well. The post processor system is very robust and easy to work with to customize. The tools are easy to use and there are a lot of tools Bobcad simply doesn't have such as automated tabs and the ability to select the start point. Other things are missing or don't work quite as flexible as Bobcad (such as won't do a rough then finish pass for profiles, but does clear out pockets and follow with a finish pass), but for most 2d work I find that EstlCAM is a bit more efficient to use. There is a demo available, but really for $25 it's hard to go wrong with it and I think it's cool to support individuals who create good products with new ways of looking at these things. Coming from Bobcad, you can learn EstlCAM in a day no problem, if not a couple hours.

[Ben S]

Thanks for outlining the work-around mmoe and I am downloading the EstlCam demo now. I appreciate the help.

[mmoe]

Thanks for outlining the work-around mmoe and I am downloading the EstlCam demo now. I appreciate the help.

No problem. Keep in mind that EstlCAM is very different in how it looks, but that shouldn't be confused for it not being any good. I may see if I can put together a quick video of how it works, but I'd also recommend watching the video the developer made as well. Just keep an open mind, it's not like other CAM systems in appearance but it's quite capable. Part of what makes it look odd (compared to most CAM systems) ends up making it easy and fast to use.

[Louis Roy]

Hello all, I am probably to late with a reply but I will anyway. One thing I noticed was the finish tool lead in was vertical, from my experience a vertical lead in is not the right way to go if you need cutter comp, it allows for no movement to activate cc. Also under finish patterns, comp setting are system comp on, machine comp off, using these settings BobCad is going to offset the toolpath for half the tool, but not give you any adjustment for the machine. System comp off, machine comp on, will give you G41/ G42 but not with a vertical lead in try one of the others parallel, right angle or circular.

I used V25 and the generic HassVF mill post. I don't have V24, so this may not be a valid answer for this question. I hope this helps.

BobCads cutter comp system was very hard for me to figure out, the V25 Mill Training video series disk 2 video # 88 at about 5 minutes in explains it pretty clearly