Thermwood Users

[Chris Robinson]

Hi, I'm a new user of Mastercam. We have a Thermwood Model 40 with 5x10 table.

 

We purchased Mastercam through our local dealer and they are great to work with. But we're having trouble getting the post to work correctly.

 

If there are any Thermwood users out there that have Mastercam posting correctly, I'd love to compare notes.

 

Our controller is a Model 91000 Super Control and Rolling Nest uses macros M999 and G901 to calculate the location of the part relative to the part fences vs the machine home (Opposite corners). When we post, Mastercam isn't locating the part off of the part fences, but rather out in space on the table.

 

Anyway, if you would like to compare notes, I'd really like to talk to you!

 

Thanks,

 

Chris Robinson

[medaq]

I have never ran the machine, But can you edge find the part. And get your position from the control. Then move the part in mastercam to the correct position, and regen it?

[Chris Robinson]

Medaq,

 

Yep, I can find the part's edge with the control. But in Mastercam, would I have to move the part away from the WCS 0,0 that amount and then regen?

 

It would be nice if the post could do all of this without adding in even more chances for error.

 

Thanks,

 

Chris Robinson

[Bill Craven]

You could enter the part's edge values into the origin fields under the T/C plane options and it will shift the numbers in the final code by whatever you enter. I find it much easier use fixture offsets: G52L# (where # is from 1 to 99). Be wary of the G53 command, I understand it does the same thing as G52 except it goes there NOW rather than wating for the next command.

[crazy^millman]

Do a search I have covered a smallbook on these very subjects.There were over 300 links but here are 2 one given some example stuff about posting the other a sample part I did:

Link 1

Example of 5 axis part I did.

 

Read the book then throw the book in a draw unless you need a code or something. 5 axis on a Thermwood is not that hard but need to remember it is a router not a milling Machine. It will do very awsome work but not milling machine type of work it is a good fast machine very capable with the right post and mind set but not something done overnight so if the people have promised part off this week they are going to need an education in what the machine can do. Get a post and your life become easier. Also James has a neat trick with point at the Top of the Zplane for the part that are very good do a search for that.

 

Good luck be patience and it will come to you. MPGEN5AX will work on a Thermwood but needs tweaking the MPMASTER_THERWOOD post was a bunch of stuff from alot of different people and got my through but could have been better oh well gave it my best.

 

 

HTH

[Snaglpuss]

Chris,

Are you just trying to drop the parts on a sheet

that is on the pop up pins or a home made fence?

If thats all you want to do then use the machine to find the coordinates of the machines table corners and the line of the fences, draw up your

machine and tables in mastercam,then save it as a drawing templet. Draw up your parts, merge in the drawing of your machine and fences, drag or translate your parts in and do your toolpaths.

Post your file and your code and you wont need any fence or other offsets to worry about.

Simple, fast and easy.

[Chris Robinson]

Mr. Craven, I got word from Ken that you guys talked. He forwarded the post and sample file to me. I read up on the G52L# and understand what you are talking about. I'm still a little foggy on what the c-plane, t-plane setup, but I'm going to talk to Ken first thing Tuesday morning. I appreciate your help very much.

 

Slaglpuss, I have a 3-axis Model 40. You're correct. I want to drop parts on a sheet that is located on the pop up pins.

 

I have already used the machine to find the location of the pins in x & y axis. Xaxis distance to fence #1 is 121.0645 and Yaxis distance to fence #1 is 66.6205.

 

I'm not totally clear regarding drawing up my machine and tables...

Could you please explain in a little more detail? I'm sorry about my ignorance. I'm still coming up the learning curve.

 

Thank you all for your help. This website rocks!

 

Thanks,

 

Chris Robinson

[Snaglpuss]

Chris,

What I ment by drawing up your machine is draw

a rectangle to represnt the table. Get the coordinates of the four corners of the machine

table and use those numbers to draw a rectangle that represents your machine table.

 

Then take that rectangle and draw a vertical line at 121.0645 to represent the fence at the short end of the table. Draw a long horizontal line at 66.6205 to represent a longer fence line running the lenght of the table. Trim the two lines together at the intersection. You can then draw

a 48 x 96 or 49 x 97 rectangle in the corner of the fence to represent stock sheet sizes. Drop your parts in the box and away you go.

 

We dont use the pop up pins here, we have pcs. of 1/4 mdf screwed down to the table with a gap in the corner to keep the crud out. We put the fences

down past the fence lines drawn in Mastercam and then use the machine to trim the fences so the jive 100% with the drawing templet. This is very fast and simple.

 

Machinist dudes reading this are probably shaking their heads by now but cutting wood and plastic sheet goods is a different thing thang clamping chunks of metal in vises and using a part offset.