BobCAD V25 Post Processor Editing - How to force no decimal on some addresses NOT ALL

Hello All,

I have a problem with the Fanuc 18T post processor for BobCAD V25. When outputting G-code for G74 Drill Cycle the post processor, as downloaded, has two main problems. The first problem is some addresses it outputs for G74 are incorrect. It outputs addresses I and K when it should be P and Q respectively.

Example,

N08 G74 X0. Z-.2301 I0. K0. R0. F.002

I think I have corrected this by editing lines 815 and 816 in the post processor as follows:

815. Prefix for Groove Cycle depth of cut? "Q" (this value was "I")
816. Prefix for Groove Cycle peck increment? "P" (this value was "K")

HOWEVER, the second problem remains. And, that is the Fanuc 18T will NOT allow some addresses to contain decimals! Of which Q is one of them. How can I force the post to output a value for Q in tenths, i.e. instead of 0.1 use 1000?

While I'm at it - Is there any DETAILED documentation available that describes the function of each line of the post processor? I thought I had found this once before for V23, but apparently I was dreaming as I can't put my hands on it.

Regards

The documentation was improved in V26. I can't say for sure if V25 has this function but I recently stumbled upon this doc in my V26 folder. It describes exactly what you are trying to accomplish.

Look in your "Posts" folder for documentation of the post variables. They are also available from the online help.

Quote:

---

Originally Posted by WCIS

While I'm at it - Is there any DETAILED documentation available that describes the function of each line of the post processor? I thought I had found this once before for V23, but apparently I was dreaming as I can't put my hands on it.

Regards

---

Sorry, missed this bit. To my knowledge there isn't any detailed documentation of each line of the post, other than the descriptions of the posting blocks in the post itself. I attempted to put one together with the help of the forum once but I was already familiar with the posting engine and it didn't seem like anyone else was interested.

Thanks SBC Cycle,

I did find that file and it is helpful to a degree. However, just my luck, the variables I need to modify ARE NOT described! I will poke around the BC website later to see if maybe there's an updated version of that file. I know many are self explanatory, but I was hoping there was something somewhere that had a little more than a one liner about each variable.

I played around until the wee hours this morning trying different things, but I believe it's a lost cause as far as the 'no decimal' allowed problem goes...

Quote:

---

Originally Posted by SBC Cycle

Sorry, missed this bit. To my knowledge there isn't any detailed documentation of each line of the post, other than the descriptions of the posting blocks in the post itself. I attempted to put one together with the help of the forum once but I was already familiar with the posting engine and it didn't seem like anyone else was interested.

---

No problem.

Yeah, once you get the post working you seem to just let it lie and move on to other problems. Unless you have an incentive such as a machine dealer, etc. there's not much of a reason to go very deep into it. I don't want to get into bashing here, but one has to pay for support, I understand that position. On the other hand why should the customers collaborate and create documentation for free?

Try changing the post line similar to this:

n,"G74",groove_x_bottom,groove_z_bottom,'[4T]',groove_peck_increment,groove_depth_of_cut,groove_r value,rough_feed

I fiddled with it in V26 and that seemed to do the trick with my post processor. I don't know if I put the '[4T]' in the right place but it should be right before the variable you are trying to format.

Of course it could be that V25 did not have this function :(

Quote:

---

Originally Posted by WCIS

No problem.

Yeah, once you get the post working you seem to just let it lie and move on to other problems. Unless you have an incentive such as a machine dealer, etc. there's not much of a reason to go very deep into it. I don't want to get into bashing here, but one has to pay for support, I understand that position. On the other hand why should the customers collaborate and create documentation for free?

---

Support is always a touchy subject. I think I will try staying away from that subject for a while. The only thing I will say is that the support here has been more than enough for what I need.

I agree, once my post was nailed down I've forgotten a lot about how it works.

I've pulled out my install CD's and I've been poking around in the files on CD and what's on the HDD. I can't find what seems to be what you have. So, I'm going to study what you gave me and I will give the variable formatting a try. I'm not sure as I haven't tried a program transfer to the Fanuc 18T, but I believe it's going to choke on the five digit program number as well. If so, I hope the variable formatting will help there too. Thanks for your help!

Okay, I found this on the BC website. Hopefully they won't mind me posting a link:

How to change the decimal format in the post processor - Powered by Kayako Fusion Help Desk Software

Also, there was a link to a .pdf - not like yours, however.

No problem. The differences between V25 and V26 are minimal but the variable formatting may be one of them. Sometimes the "Version" number of your post can make a difference also. In my V25 folder the posts have revision numbers of 1.1 and 1.2. In V26 the Version is 10.0:

Code:

---

****Version number MONTH DAY YEAR****
1000. Version Information = Version Month Day Year? "10.0 09 25 2013"

---

What does it all mean? I don't know!

At least changing the number of digits for the program is easy. To change the number of digits in the program number check Block 302 (for lathe):

302. Number of places for program number? 4

Interesting. I had not seen that document before. <right click - save>

Thanks for posting that.

It would appear from the date that it was posted that this should be available to V25.

That formatting deal WORKS on the variable I needed to modify, i.e. groove_depth_of_cut! What's interesting is you MUST surround the format specifier in single (or double) quotes. That tripped me up as I'm used to programming documentation that tells you to omit those. But, NOT here!

(I deleted a stupid comment here as I didn't read well enough earlier.)

As far as post versions I downloaded the version I'm modifying from their site just after the V25 upgrade. The version is 9.2. I had numerous errors in the G-code output right out of the box, so I really don't think too many people are using it if any.

Thanks again for your help!

Quote:

---

Originally Posted by SBC Cycle

At least changing the number of digits for the program is easy. To change the number of digits in the program number check Block 302 (for lathe):

302. Number of places for program number? 4

---

Yep. I should've had my eyes open, too!! I didn't notice this earlier. Thank you for that little pearl of knowledge as well!!

Sweet, glad it worked. The formatting with the quotes is definitely odd and the two pdfs seem to conflict. It just took someone who needed it to work to get it squared away. This may come in handy for me as well. One of the only things I still haven't got quite right in my post is how to force high gear when rigid tapping in the Fadal. It requires a .2 after the speed like this:

S820.2 M3

This might do the trick. A useful discussion for me as well.

Yeah, I've got the same issue. Not sure if this will help you, but it's what I did to work around the problem in V23. It DOES NOT fix the problem, but merely adds a note reminding me what needs to be done. I also use .400" clearance as a safety prior to moving to the next hole just in case something isn't quite right with the feed rate. The following are a couple excerpts from the V23 post that I use:

74. Left handed tapping canned cycle.
rigid_tapping_start
n,"(set hi range spindle above and 0.4 inch clearance height for Z above and R below)"
n,default_add_spaces,g_canned_cycle,g98_g99,x_f,y_ f,drill_depth,reference_plane,tapping_feedrate,s,f orce_no_add_spaces,".2"

84. Tapping canned cycle.
rigid_tapping_start
n,"(set hi range spindle above and 0.4 inch clearance height for Z above and R below)"
n,default_add_spaces,g_canned_cycle,g98_g99,x_f,y_ f,drill_depth,reference_plane,tapping_feedrate,s,f orce_no_add_spaces,".2"

This isn't perfect, but it works well enough that I just got used to it. I find myself tweaking the G-code a bit anyway after posting so it's just become habit.

By chance are you also posting for a Fadal?

I will admit, I did not think about simply hard coding a ".2" after the spindle code. That would have been much simpler than the craziness I used for a long time to accomplish the same thing. With my later attempts I was able to preset the spindle speed right after the tool change (to keep the machine from switching to low and then back to high at the tap line) but there is an error in there that I haven't taken the time to track down and I just need to find a better way.

I also like to start my rigid tapping with a greater clearance plane over the hole than I do for the spotting and drill cycles. I resorted to separating the tap as a completely separate feature so I could set a different clearance plane but it makes for twice the work. Sounds like you are running into the same problem?

Yep, SBC we are both having the same issue. Although I do have seats for V25 the guys and I normally stick to V23 for the two mills. One of which is a Fadal with CNC88 control. We use it in format 2. Everyone has access to V25, but V23 seems to be the version almost always open on the dev computer.

When I need to tap holes I just go with the .100" clearance plane default in the feature and tweak the code after the post. Hence the reminder comment in the post. I don't completely recall as it's been a couple years, but if memory serves I couldn't use the 'hard code' scheme to add the .2 after the spindle speed variable at the top ** of the feature as it would keep the spindle in Hi gear for other operations. So, that's how I ended up with the post processor as it is now.

N34 (TOOL #5 .315 SPIRAL TAP)
N35 T5 M6
N36 G0 G90 G54 X.2862 Y-.4232 S472.2 M3 **
N37 G43 H5 Z.4 M7
N38 G84.1 G99 X.2862 Y-.4232 Z-.6469 R0.4 F23.2285 S472.2
N39 Y-1.1516
N40 X3.7137
N41 Y-.4232
N42 G80

This G-code fragment has already been cleaned up a little, but my reminder comment would show up between N37 and N38 (if I remember correctly). Then as I go through and remove all the extra S codes, F codes, G90's, G54's, etc. I will add the .2 to the S code at the top **, change the initial Z position to .4 (@ N37), and change R0 to .4 (@ N38) then delete the comment (as my marker that it has been taken care of). I'm not at the shop now otherwise I would generate a post for you (without edits) and put it up here for you to see.

(I pull out the extra S and F codes to make it easier to tweak those parameters during G-code proofing. I remove the other extras just to get rid of the clutter for ease of troubleshooting.)

This is something to revisit I think. Maybe the answer lies in these sections of the post processor:

20. Spindle speed low range

21. Spindle speed high range

22. Rigid tapping start.

23. Rigid tapping end.

.