Tool Numbering problem in X9

[Code_Breaker]

I have a tool numbering problem in X9 ... first time ... see attachments

 

 

1)  Tool Manager and Tool Library has one set of number, both the same.

2)  Toolpath Manager, the tools has the same numbers ... no differences

3)  In the NC files, they are different

 

Why? I cannot fix this, tried several times. I have been using here since last April using the same library, tools with these numbers, same post. Also, on another computer with a different post, I am getting the same problem.

 

Can anyone help?

 

Don Dawson

Corona, CA

 

 

[gcode]

Look on the Tool Setting Page in the Toolpath Manager

See if " Assign Tool Numbers Sequentially" is checked

 

Also, review the settings on the Tool Page in the Control Def

[Code_Breaker]

Same Machine and Control Settings, Same Post, Same file.

 

I had to make three similar vacuum fixtures which I used the same file for all three, but were under different jobs so three files made from the first as a Seed file.

 

FXT-1 and FXT-2 were OK, FXT-3 was the problem. All three used the same tools.

 

Don Dawson

Corona, CA

[BrianP.]

When I have seen funky stuff happen I have had some success with running the RAM saver and/or doing a rename  NCI.

[Colin Gilchrist]

Have you tried forcing a Regeneration of the operations? I'm with Brian, I'd recommend running RAMSaver and also just doing a Restart with Mastercam.

 

Also, you can try selecting a different tool, regenerating the operation, and then re-selecting the tool you actually want, and that should flush out any "bad data" that may be hanging around.

 

One thing I would recommend is checking your Operation Defaults file, and making sure "Assign tool numbers sequentially" is turned off in the Defaults file. Then check and be sure that isn't turned on in your current Mastercam file as well.

[Code_Breaker]

Did anyone look at the pictures? Are they hidden?

 

Picture-1...Shows the Tool Manager with Part and Library ....these tool numbers are correct

 

Picture-2... Shows the tool number (primarily 13, 18, 19) ...these tool numbers are correct

 

Picture-3...Shows the Tool List generated by the post...Tool #13 is correct, while Tool #10 & 11 are wrong.

 

Picture-4...Shows the NC Code for T10 (T18) and T11 (T19)

 

Also, the "Assign tool numbers sequentially" is not checked (You can see that by Picture-3)

 

I wrote FXT-1 and FXT-2 yesterday morning, and they ran perfectly, I copied FXT-2 and renamed it FXT-3, stretch the geometry to be about an 2 inches longer... regenerate toolpath and posted last night.

 

I turned off my computer and went home.

 

When the operator saw the numbering didn't match, he told supervisor who opened it on his machine, re-selected all the tools and regenerated them and re-posted with a different post. Still wrong.

 

When I got in, I was told what happened, so I open the file, will select every operation tools--regenerated--re-post ... same problem.

 

When you open a file, no need for RamSaver...you will get the message "Database Did Not Need to be Changed."

 

If you want, I made a Zip2Go ... it is attached

 

Don Dawson

Corona, CA

 

 

 

 

COVER_FIXTURE-3.Z2G

[gcode]

There is no Mastercam file in the Zip2go

[Colin Gilchrist]

Yes Don, I looked at your pictures. There is obviously something screwed up in the Binary Operation Data, and how it was stored. I say this because you had 2 programs that worked fine, and this 3rd one is exhibiting this strange issue. Since RAM Saver doesn't see any change in the "path" or other parameters, it doesn't see anything that needs to be "fixed".

 

Have you tried switching tools, regenerating, and then switching back? That's about the only advice I can think to give, other than you should probably send this into CNC Software (the MCX file) as a bug. That's what it looks like to me. I know that doesn't help you figure out how/why it is happening, but hopefully it could help solve the issue.

 

You've got bad data that is making it into the NCI somewhere. Looking at the Tool Manager doesn't really help in this case. Why? Because the Tool Data that is output in the NC Code is stored in the Operation data structure. Although you've got the "correct" tool data in the Tool Manager, and it displays correctly in the Operations themselves, when the Binary NCI is converted to the ASCII NCI, the wrong data is being written.

 

Changing the tool in the operation and then regenerating (with an admittedly "wrong" tool) will force the Operation to be written using this new Tool Data. Then changing the tool back to the "correct" tool will then show a "change" and when you Regenerate, it should force Mastercam to write the correct Tool Data to the ASCII NCI, and give you good code output.

 

Why is it happening? That's not something I'm able to truly diagnose, which is why I recommend sending this file (a copy of it before you fix it) to CNC Software as a bug investigation.

 

As a test, try going into the Operations Manager, selecting all operations, then holding CTRL + ALT + SHIFT on the keyboard, and Right-Clicking on the selected Ops. There will be some additional options that show up in the Right-Click menu. Choose "dump Binary NCI data". (I think that's what it is called. I'm not in front of Mastercam to be able to test it...)  That should dump the Binary Text Data, and I bet you'd see that "10" and "11" are set in the binary NCI for those particular operations...

[Code_Breaker]

Thanks Colin, that worked ...

 

Also, in the zip2go file included the data path as well. The MC files is under "Manufacturing>Machine Shop>PROJECTS>VACUUM PLATE>MASTERCAM"

 

Don Dawson

Corona, CA