CAMWorks problem on Haas TM1

[riveter]

Hello.

I am learning use CAMWorks on the Haas TM1. I am experienced on the Bridgeport manual mill and manual lathes. I am new to the Haas.

I have a post processor file that was given to me by one of the designers. It shows that it is a post for a 'Sharp' machine with a 'Fanuc' controller. I don't know where he got the post file.

With CAMWorks I am having trouble with 2.5 axis programming, specifically cutting bosses (any feature that protrudes from the part face). The CAMWorks simulator shows a good part, but when I run the program on the Haas, it cuts off the corners of the adjacent boss. I was using a 3/16 inch endmill and the cut is 1/4 inch wide, meaning the tool ran an offset path that I did not program it to do.
I sent the part file to CAMWorks tech support. They posted it and looked at the G code and said it looked fine. They asked what my G41 setting was. All I know to check is the 'wear' value for the tool diameter in the tool offsets page. That value is '0'. And the diameter is set for '0.188' which is correct.

The CAMWorks tech said my problem is either a bad post processor or a bad setting in the Haas.

The designer who gave me the post file looked at my bad part and said "cutter compensation".

My question is: Where do I check cutter compensation in the Haas controller?

Can someone tell me how to get a good post processor for the Haas TM1 with tool changer? CAMWorks charges $250 dollars for a post processor for licensed users of their software.

Thank you for any light you can shed on my problem.

[bsuchland]

CAMWorks don't directly charge for all their post processors. The resellers sometimes charge for them, based off of the number of hours the put into writing and developing the posts. Some posts take hundreds of hours to write, so they offset the costs of development time to selling some of the posts.

It sounds like to me your reseller gave the wrong post either that, they gave you a post that was intended for a Haas but didn't update the name in it the source files.

However, I do not believe that either of these are your issue. When the "diameter" of the endmill is defined on the machine, the machine will typically then offset the XY values it reads from the post by the tool radius. CAMWorks has the option to offset those posted XY values by the tool radius or not. I am speculating that this option is being offset by both CAMWorks and your machine. You only need one or the other to do it. This can be achieved by not entering a tool diameter (maybe a zero diameter) on the machine or when within the CAMWorks Contour Operation, go to the NC tab. There is the option to turn on or off toolpath center compensation. I am guessing you have this on... this means CAMWorks is offsetting the XY values for you. Turn this off and then it won't do that. (Basically draw a simple square, post it. change that option and post again. you will see the difference in the posted XY values).

[riveter]

We paid CAMWorks for a post processor for the TM1. It has been working great.
But yesterday I was cutting an open pocket with an island in the middle I let AFR define the operation for the pocket and it looked good on the simulation.
It properly cut the pocket, but comped the cutter when cutting the island and made the island too small by what looks like a cutter radius on each side.
My question is what is the proper way to fill in the cutter page on the Haas. I have been entering the tool diameter and setting wear to 0. Should I set the tool diameter to 0? Since CAMWorks knows the tool diameter, does it need tool diameter to be entered in the Haas controller?

[extanker59]

You can go either way. Just need to make the settings in CamWorks the same across the board.

But, since this will affect many operations, I suggest you leave your Haas geometry at zero to start. When you need to comp the tool, put it in the geometry section not the wear section. This was told to me by a Haas aplications guy. Don't remember why he said not to use the wear section.

[hoganj]

I have a TM-1 and use camworks. I have all my diameters set to zero. than if I need to adjust a boss or a pocket you can add in +/-.001 for example to compensate. Your post is probably fine. By default camworks ads 20 to your diameter number. For example if you are using T10 then your Diameter will be D30 in your code. So if in your tool offset menu on the TM1 you have a diameter set for D30 and the code calls for cutter compensation than it would offsett what ever you have set in D30. You can change this setting in the Universal Post Generator that is usually included with camworks. I have a lot of excruciating experience with camworks and its little pecadillos so feel free to ask
Jake