You can get volumill with bobcad if you want, or get their standalone product. When they approached me to Rep their software I chose not to cause for the money I saw no competitive advantage for my customers. I also looked at all the third parties over the years that have come and gone and did not want to go down that road. (again) Maybe cnc's deal was that they came out with a standalone product which would make them a competitor. Who knows? I do know my mastercam customers are eating everyone else's lunch without it

Roger I would like to know more about the new functionality if you could send me some info on where to look. Will it work with scripts or just nethooks?(I unistalled .net and went back to studio a couple of years ago. DOH!)

I like having the post forum so its easier to find the post topics. Both options sound like they are "for" a post forum also :headscratch: One of the many things the post development team is working on is to make posts simler. Or atleast the parts end users want to tweak. Most post writers got to the point their at by picking up from things from other people and adding to them. When I started using Mastercam 20yrs ago there was no one to ask about posts. I would change on thing in the post, save it, start Mastercam, post something, see what it did, close Mastercam and repeat process. (Gotta love the old dos days) I did finally meet Rich Taft and Jeff Hill that worked in the post dept back then. Finally someone to ask questions. Then the Mastercam 5 post book came out. That was extremely helpful. Now between CNC Software and Inhouse there are 10-20 full time post guys, and customers have access to them in one spot. BTW the full time guys don't just work on posts, they are responsible for updating, linkage, nci file and future development as well. This forum gives them a resource to use as they are deciding what overall direction posts should go in. The beta forum is great for all things Mastercam, but the post is the most important part of the software. If you don't have a post, there's noway to turn the bluelines in backplot into good nc code. Having a post forum is something that was long over due imho.

Ex, Do you always add 10 to the lentgh offset each time it is used? I done a haas(think it was a haas) post like that that awhile back. I like the notification so I can fix it in the mcx file.

You could change it in the toolchange section of the post, depending on the type of cut may not be what you want everytime. Instead of changing the post you could use points to move the tool to Z(whatever) then do your od operation. You could also use points to drop X first for id ops. To create the "goto " points use toolpath- point.

Depending on the post you start with you my have to put it in psof$ as well as ptlchg$ section. What I do in the haas post is add tlngno$ = t$ and that always makes it equal to tool number. If you want an alarm from post there's a few more steps #Declare a string varible to output to screen and dummy varible s_offset_err "Height offset does not match tool number!" err_off : 0 # dummy varible to test output #then add to ptlchg$ and maybe psof$ if tlngno$ <> t$,[ err_off = mprint(s_offset_err) tlngno$ = t$ # to automatically change it #exitpost$ # if you'd rather quit processing and fix in mcx (you have to remove#) ]

Mark have you tried using the highfeed option in Mastercam? It does exactly what your wanting. It will break lines as it approaches a corner stepping down the federated, then accelerate the same way.

In the older surface paths you need to set "depth limits" on last tab of operation On newer surface paths its set under "cut parameters"- "steep/shallow" For 2d paths you have to turn depth cuts on in order for them to reckonise the top of stock setting. HTH

Inorder to program the grinder I suggest using a slot cutter with full rad to represent the grind wheel. Should be able to program the part that way. A 5ax grinder will require a custom post though.

The cms aries is a very nice machine, but as you stated, not a machining canter. If you have air blast you can rip thru some aluminum though. Does it have the fanuc control or the osai control? Usually the aries has the fanuc on it, just making sure. Inorder to machine it the way you want to just click on t/cplane at bottom of screen and set to "Front". Then you can use any 2/3 axis path you want just like you always have. Note: All 5 axis paths need to be programmed from top cplane as a general rule.

Are you using the y axis on machine or the c axis? If your doing the path in the right cplane then your x is going back z into part and y is up and down. send me a sample file your trying to do andthe post so far to look at along with desired output if you have it.

The standard ultimax post should work fine, typically I send my customers the v9 post and they just update it. It even works on the new hurco control. Do you know if thats where yours came from? As far as post editing. Alot of things are handled thru either machine def or control def, and when I have to edit the post I just use notepad.

Also, I got the idea that you were just wanting this post to use for the situation you mentioned. This is just a "down n dirty" way of doing what you want. To incorporate this into a lathe post there is some logic we'd need to add.

Oops Do not change: fmt X 2 xabs to fmt X 2 xabs_dia But... add fmt X 2 xabs_dia like: fmt X 2 xabs fmt X 2 xabs_dia Also in the pfxout and pxout post blocks instead of outputting xabs you want to out put xabs_dia

Here is a simple way of doubling x at the point of output. . You have to also add the xabs_ dia variable.(Note it will not work with incremental values without adding more logic.) fmt "X" 2 xabs_dia pfxout #Force X axis output xabs_dia = xabs * 2 if absinc$ = zero, *xabs_dia, !xinc else, *xinc, !xabs pxout #X output xabs_dia = xabs * 2 if absinc$ = zero, xabs_dia, !xinc else, xinc, !xabs

If it is doing it with the default post it would have to be the computer, but that really doesn't sound right. I don't know of any settings in Mastercam that you could set that would "ignore strings that start with a space" Maybe something to do with anti-virus, but again that really don't sound right. Anyone else have any ideas or seen this?

I tested putting a space in front of the tool string and operation comment and both were output in the gcode with the space no problems. What version Mastercam are you running?

There's alot of good dnc software out there. I'd say the top 3 are cimco,extreme dnc and predator. Just make dure whatever you go with meets your specific requirements. The bigger issue to decide is what hardware to use. Straight rs232 from pc with multi-serial io board Network multi-serial io and rs232 Single port serial to ether at each machine Or wireless I think currently the most reliable is single port to ether adapters at each machine, but wireles has come a long way and is a close second (of course its a little more pricey.)

I used to use: if xinc <> 0 | yinc <> 0 | zinc <> 0, feed_chg = 0 ..but changed the format to make it easier to read.

If I understand correctly you want it to change feedrates if only a rotary axis is moving by itself.(?) Maybe an easier way to do it would be to test xinc,yinc and zinc to see if any of those are moving. Maybe add something like this to pfr$ feed_chg : 0 pfr$ feed_chg = 1 if xinc <> 0, feed_chg = 0 if yinc <> 0, feed_chg = 0 if zinc <> 0, feed_chg = 0 if feed_chg = 0, feed_out = fr_pos$ if feed_chg = 1, feed_out = other_feedrate

If you feel comfortable with it the next step is to dryrun on machine if the control has that option or just raise the offsets up to a safe distance and test run keeping feedrates/rapids turned down and thumb on estop.

When declaring numeric variables you have have ": #" to do so I always use spaces between operators. The following will always make my_var = 1 since it resets to 0 at the top of post block I wasn't sure what "counter" was doing. if its a call to a post block it needs to be pcounter as postblocks must start with letter p my_var : 0 counter_int : 0 # initialize variable p_some_post_block my_var = 0 #counter ----not sure what this is my_var = my_var + 1 *my_var, e$

I would start by taking a v9 mc9 file and posting it with mpfan. Compare the nc file that v9 created to the one that v5 created and see what the differences are. If the machine is pretty standard you may only have to do some tweaks to pheader, tlchg and peof. Just be sure and start with a good nc file.

You can use the while function to do this my_var : 0 post_block1 my_var = 3 #set varible start value while my_var > 0, post_block2 #loop post_block2 my_var = my_var - 1 # counter *my_var,e$ # do something I sometimes forget to put the counter in the 2nd postblock and that cause the post to run an infinite loop

Keith what was the "post work" you were wanting to do. Maybe there's another route to get there. Maybe set up min_limit_c and max_lim_c and in pcout/pfcout: pcout/pfcout if cabs < min_limit_c, min_limit_c = cabs if cabs > max_limit_c, max_limit_c = cabs If you needed it at top of nc you could write everything to subout = 1 then in peof switch to subout = 0 put limits in and mergesub? Colin, I never noticed the .ops file wasn't there any more. Memory map is basically the same thing then, just available at run time?