MCX Importing operations to a new graphics file

[Gramby]

Frequently I have parts that are similar. Not a mirror, but only similar. The tools and operation required to do the parts may be the same or very close. I program one complete. I then bring up my new file for my second part. To makes things quicker I right click the operations manager and select "Import" to import operations from my first part. I then only need to select geometry. Tools and depths are already their.

Here is the problem. If I have two tools the same dia. it uses the first tool used for both operations. Example if operation #1 T5 is a 1.000 Rougher and operation #2 T10 is a 1.000 Finisher. When you import the operations, operation #2 will T5 a 1.000 Rougher rather then T10 1.000 finisher like it should be.

It appears this happens because the dia. are the same and mastercam import is using the first one for all operations with that dia..

Does anyone have a solution? I relize you can go in and select the correct tool. But it can be easy to over look and you expect it to be right in the first place.

[peon]

WARNING!!! I just did the same as you for the first time last week and the tool length offets weren't transfered. It defaulted to an H0. I didn't notice it till I slammed a ball mill into my part. Keep an eye on that. I also have the same problem you described and I hope someone here has a solution too.

[Rick Henrickson The Boeing Co.]

isnt there a check box, and you have to open the ops and click on the tool to get the h and d value to match, I don't know how to get around it

[?Mark]

quote:

---

Does anyone have a solution?

---

NO.

It's been talked about several times, most recently here.

 

Which reminds me, I was supposed to setup a poll to see what the general consensus on this is and hopefully get cnc folks to work on it a liitle more

 

[peon]

I never have a problem getting the h and d value to match in all cases, except when importing the toolpath.

[Gramby]

Mattstang thanks, you are absolutley correct my height offset and tool dia. offsets were wrong. Appears as though opening the operation and clicking the tool required resets them correctly. That said, importing operations is very high risk. Which is a shame.

 

Thanks Again

[dantheman]

I only mess with importing ocasionally but as i recall you have an option when you import to "disable duplicate tooling" I use this to avoid having tools of the same dia. being deleted! You also have some other options as i recall

[Gramby]

Dantheman you may be on to something their. I never saw the "disable duplicate tooling" selection before. If I would have ,I would of thought it meant duplicate tool #, not tool dia.

If any one sees a method to keep this defaulted with a check, please let me know. Can't think of a reason why mastercam would even put this here.

It now appears to import operations with the correct tools assigned for each operation. The only problem now may appear to be what mattstang70 shared. That is if you open up your tool operation your length offset and dia offset will not be correct, it shows "0". When your at this postion if you click the tool it will reset this value.

Ideally we shouldn't have to do this or even open this page. We should only have to select new geometery and regenerate without ever opening the operation.

Hey were halfway their.

[dantheman]

Out of force of habit i will often go to the "edit selected operations" than "renumber tools" to get my off sets and values set properly. This only takes a second and usally sets every thing! To be quite honest I will not even bother checking if they are right or not because i have been burned once! The guys on the floor, thankfully are awake enough to catch it!

[Gramby]

Sounds like a good method for those who use tool numbers in sequential order. Unfortunatly mine are not, are shop tool pods are assigned a particular tool type.

[dantheman]

Just by the by I noticed in system config under tool paths there is an option their for "use existing tools" when importing operations? Maybe that might help out? Like i say I never use import enough to to chase down the problems!

[Gramby]

Looks like a possiblity, I looked at my config. and I already had it checked. I searched for what exactly this does and found the following.

 

Quote:

 

Check this box to use tools already in the tool list that match tools required by an imported operation without asking the operator. Clear this box to always ask the operator first.

[Gramby]

Warning: On a import of operations which include surface parallel paths you will also loose your step over distance that you initially had. Just got a bad reminder.

Now that this happened I can remember once way back when I lost my step down amount "Depth Cut" on a 2d contour.

Bottom line on a Import of operation's go thru every operation and check all the values once again. Till mastercam fixes this.

[dantheman]

okday Gramby I might have something for you. Before you import the operation go to your stock setup- tool settings. In there you will find a seting for asigning tool numbers sequentially. Turn that off and it brings the original tool numbers in! Now the question is can that be set inside of config?

[dantheman]

Just to add something further, there is also an option in advanced options about over riding model with default values! It lets you keep clr. height etc.