Backplot Cycle Time Calculation

[BK]

This not a huge issue as I have a post that I will use occasionally just to get an accurate cycle time for a program but I have noticed that when running backplot, the software is interpreting the dwell (on a G82 spot drill cycle)as a value of seconds. The control reads this value in milliseconds (P30 for example).

 

The Backplot function sees that as 30 seconds, little difference there.

 

I usually use a dwell value that will let the tool dwell for 5 revolutions when it reaches the Z target. With a high load operation like spot driling it helps to unload the tool and servo before heading for the next hole.

 

Just wondered if maybe there was a cfg setting that I was missing

 

Thanks in advance,

Bob

[Mike Whitten CAD/CAM Contractors]

BK,

quote:

---

Just wondered if maybe there was a cfg setting that I was missing

---

I have never heard of one but there are other people who know this software better here than me.

 

If this is the case, send it to [email protected] and get a bug number. If nobody logs it, it will not get fixed.

 

I also use G82 on spot drills and other tools but normally I have between .1 and .3 seconds. I think you generally need just enough for an "exact stop" but sometimes as you say more is needed. I need to look at this also because maybe this has something to do with my incorrect times.

 

Thanks,

Mike

[Teh Bear without Brains kinda idiot]

In your place I would correct the post ,IOW input value 0.03 instead of 30 in MC and in post

multiply it by 1000 .

I do not think it is a bug ,JMHO .

 

Teh humbliero

[Teh Bear without Brains kinda idiot]

BTW ,put a quick help sign (an icon near the X sign in upper right corner) on dwell parameter and you will see :

Set the ammount of time in seconds .....

 

HTH

WTHH

[Mike Mattera - TFM]

if your putting in the number 30, Mastercam see's that as 30 seconds. Pooh is right. You have to alter your input (.003)to reflect the REAL value you want (i.e. P30) in the output of the post. A Fanus expects the value to be represented in 1000/th's of a second. So you have to multiply is by 1000.

 

dwell = dwell * 1000

 

Mike Mattera

[Shawn Wentzel- Wenteq Inc]

I had the same problem and called CNC software and they were not aware of it. I guess changing the post would work as long as you remembered to enter everything in right.

[Mike Mattera - TFM]

The input for Mastercam's dwell parameter is in seconds. The input for Fanuc is in 1000/ths of a second. You have to enter the data right in order to have compatibility between the units. It's the only way it can work if you want the correct cycle time.

 

Mike Mattera

[Teh Bear without Brains kinda idiot]

You can change *.txt file that goes with your postprocessor to something like this

Dwell (in seconds )to remember

and selecting appropriate post file you will see it in drill operation parameters

This is from Demo MC9 help about lathe ,the same is for mill

~~~~~~~~~~~~

his procedure describes how to change the name of options in the Cycle drop-down list found on the second page of the Lathe Drill dialog box. It can be done while Mastercam is running.

Important: This procedure does not describe how to customize the post processor so that it recognizes and associates the new cycle names with specific functions that you want those cycles to perform. See your local Mastercam dealer for instructions that are specific to the task you wish to accomplish.

 

1. Using a text editor such as WordPad, open the .txt file associated with the post processor you are using (ex. MPLFAN.TXT).

 

2. Scroll, or search for, the header that represents the drill cycle you want to change. For example, [lathe simple drill]. The default text is shown below.

 

 

 

Note: There are 11 items under the [lathe simple drill] header. The first represents the description of the cycle that displays in the drop-down list. The others represent different input fields.

 

3. Place your cursor on the input field you want to change, for example [Custom cycle 10].

 

4. Change this text to read ["Drill Counterbore with Dwell"].

 

5. Choose File, Save, then close the text editor.

 

6. Open Mastercam, or if Mastercam is open, choose Main Menu, NC Utils, Post proc, Change.

 

7. From the Pst directory, choose the post you just edited (ex. MPLFAN.PST), then choose Open.

 

8. Access the Lathe Drill dialog box and go to the Cycle drop-down menu on the second page. The text changes you made are reflected in this list.

 

Note: You can change any cycle option in this drop-down list, not just custom cycle options. However, if you change the description for a field, the value for the field is still written to the same post processor variable. For example, if you change the 1st peck parameter to read "Tap," the value you enter is still written to the peck1 variable when you post the file.

~~~~~~~~~~~~

HTH

WTHH

[Mike Whitten CAD/CAM Contractors]

Thanks guys,

 

I may have been unclear in my post or understanding of BK's post. I do realize that the time is in seconds and the the post must be correct.

 

Thanks,

 

Mike

[BK]

Thanks for all of the info. The value I am getting is correct for the machine (P30) is 30 milliseconds, I was just concerned with the backplot times.

 

Here is another thing, one of the few things I had to change in my Fanuc posts is this . . .

In the NC output varialbe format I had to change the line shown below . . .

 

fmt P 4 dwell #Dwell

 

I had to change to a 4 instead of the default 11 value for the formatting.

It was outputting a (P30.) and our Moris will not let you use a decimal value on the dwell cycle.

 

So it looks like I should do some calculation in the post so I can use .003 in the drill op and get a P30 in the posted code?

 

Thanks for all of the info,

Bob