Thermwood post for x some help please

[Tom m]

does any one have a working post for a thermwood 5 axis in x? we have 3 post for 9 but one well update right in x tried our reseller not a lot of help! just want to see if any one out there has one that is working! not trying to start trouble here!

 

[ 12-15-2005, 02:01 PM: Message edited by: Tom m ]

[dwsz71]

Oh boy...

[Guest]

Dude, welcome to the forum and all but bad move.

 

Read the FAQ, requesting a post is not a good way to jump in around here.

 

There is time to hit that button in the top of your post with the pencil to ask for help modifying your own post instead but if you need a new post your reseller is the person to ask.

[Tom m]

they have not been a real big help sorry if that was a bad idea if a mod want to remove it that is fine just wanted to know if any one had one or where i could get one?

[Tom m]

we have 3 of them for v9 but none work right in x if you have seen a thermwood befor they are a lil dif table only moves in y spindle is x z c and b tried updating out post but no luck

[Guest]

There a people here who are more than willing to help you get yours going but I don't think anyone is going to give one away.

 

Ask some specific questions about the problems you are having and you might be happy with some of the answers you receive.

 

 

[Allan Brown]

Are these CNC Automation posts? Have you contacted them for an update?

[Tom m]

Thats just it i dont know thy got them befor i started there and no one knows i dont know how to tell!

[Paul Decelles]

What happens when you update the posts? Error messages? Bad NC code? No NC code?

 

I've updated approx. 15 Thermwood 5-axis posts and the only problem I have seen is a blank nc file when posting. This is due to some internal logic checking the version number and exiting the posting process.

 

If this is the case for you, open the file "customize.update_mill" (or "customize.update_router" if you are updating as a router post) in your chooks folder (C:mcamxchooks) and add the following lines to the bottom and try updating your V9 posts again.

 

code:

---

// Fix an error common to MPGEN V9.00 posts

1. if vers_no < 8 | vers_no > 9,

2. if vers_no <> 10,

3.TRUE

4.TRUE

5.TRUE

 

// Fix an error common to MPGEN V9.00 posts

1. if vers_no > 9,

2. if vers_no <> 10,

3.TRUE

4.TRUE

5.TRUE

 

// Fix an error common to MPGEN V9.00 posts

1. if vers_no <> 9,

2. if vers_no <> 10,

3.TRUE

4.TRUE

5.TRUE

---

If this doesn't work, email the V9 posts to [email protected] and we'll have a look.

[Guest CNC Apps Guy 1]

5-Axis Posts will be a problem getting for free. Those are generally coded to a particular SIM and will only run on that SIM. So even if somebody were to give you one they paid for, you still may not be able to run it.

 

General rule of thumb around here though for future reference is don't ask for free posts without being here and contributing for a while, and it's never really a good idea to ask for 5-Axis posts.

 

Good Day and good luck.

 

Contact CNC regarding the matters Paul brought up and I'm sure they'll be able to at least tell you what you need to do to get going.

[Mike Mattera - TFM]

Tom, you really need to tell us "what" is wrong. A little detail will go a long way to getting the problem solved.

 

Mike Mattera

[Tom m]

ok here we go i only got one to update at all and when u post it sends codes out like a 3 axis and the machine def... is all messed up it puts x and y on the tabel when it is only y and it puts an a axis on there and b on the head when it is c and then b on the head the other 2 say they update but they dont work at all! and i am not lookin for a free post just wanted to know if any one had one that works i called CNC Automation they said it was not one of theres and they would not have one ready for at leat a week that one is 2600.

[Jimmy Wakeford from Barefoot CNC]

I have seen several issues updating 5ax posts. The machine def stuff being the least. There is a mapping issue if the old post used:

 

rotaxtyp : 4 #Rotary axis type for toolplane

 

if you can get to the section of the post where the x,y,z calcs are done you can switch it to use the matrix mapping stuff:

code:

---

pmatrix_su #Establish mapping matrix 'mmtx1'

#Machine Base is 'matb1'

tmtx1 = matt(aaxisx)

tmtx1 = mmul(tmtx1,m1)

rmtx1 = matt(m1)

mmtx1 = mmul(rmtx1,matb1)

---

,but that is sometimes said way easier than done. I only posted the "get the numbers" part of the code, you'll have to look in mpfan.pst to see the 50 or so varibles that drive this method.

 

On a "knuckle head" 5ax, getting the correct numbers is only the start of posting. Then you have to use alot of logic to allow for "over the top" B+ into B- moves, pre-wind and un-wind conditions, not positioning thru the part to another toolplane, etc.

 

There are quite a few people here that can help out if your post does not have a .psb file latched onto it. if it does then you'll have to go back to whoever wrote the original or someone at cnc software that can "unbin" the post, which they do reluctantly if it is not theirs cause the post was someone else's intellectual property.

[Brad McIntosh]

Tom's company contacted us to get an updated version of his 5 Axis post for his Thermwood CNC router. After checking our records and having him check the the post and the output from it, if appears that it was provided by CNC Software and/or one of their dealers. My assumption is that it is based on the old v8 MPTHM5 post that is on the Mastercam Extranet or on one of the variations offered by some Mastercam dealers that we have heard about over the years.

 

CNC Automation should have the updated version of our post for X ready this week. Thermwood owners should contact Thermwood's software department if they are interested in updating CNC Automation's v9.x post to the new X version.

 

If Tom cannot get his current post updated and operating correctly by his dealer and/or CNC Software, we will endeavour to work out something special in order to get him up and running with his Thermwood and X as soon as possible.