Is there a way to have the speeds and feeds that are put into a tool you create in a library automatically be put into the "Parameter" of the sequence you want to use based on the tool info? Seems like the tool has the info relative to it but when selecting the tool I want to use the data for the parameter has to be in the saved "Parameters". Sorry if confusing. Trying to create a tool library for a new machine we are getting, any tips out there for dealing with tool libraries??? Also high speed machining parameters???
Jeff Rembold did a webinar a while ago called NC Config Tips. In that webinar he explains how to setup the tool library and materials so the parameters are saved for tools.You can probably email him and get a copy of the presentation. His email is -
It is actually in the tech tips section of the ptc web site and it's called Configuration Best Practices in Creo Elements/Pro (formerly Pro/ENGINEER) Manufacturing NC Solutions. So if you have a current maintenance subscription you can download it or just wath it on the web site.
Hope this helps.
This type of functionality should be built into the software and not require any extra setup. That being said the video Steve mentioned will show you how to setup your material library and load speeds and feeds for your tools.
I agree with you nick, The tool parameter setup in Wildfire is like a house of cards. make 1 change to a tool and the parameters disapear. it should be an easy thing to work with.but it's not. I am hoping for better things with Creo Parametric 2.0
Is there a way to get the tool positition in the "Tool Parameters" to match the actually tool you want to use? When i say enter T12 as the first tool i'm using it will put it as tool 1 in my program rather than T12 when i create it. Also is there way to get the tools to show up in my program when i create it relative to the program i'm creating.
Ok the time is unimportant. So when you create a manufacturing file you create an operation and select your machine. That machine selection brings with it all of your tools that you have defined. If you want to add a new tool to that list there is no way i know of to control the tool # defaluts when loading.
I know I have the same concern. I'm lucky to almost always use the same tools in each machine with just a few misc tools.
Gotcha now! So if you set up your machine with the tools as Nick was saying they should remain in that set up for reuse with the speeds and feeds also.
Guess I don't know how to set up Machine with Tools properly it sounds like. Any help out there for this novice??
Thanks for all the support too!!!!
It's Rare for me to the same job more than once so I don't use the tools in the machine. I set my tools by operation and they are all solid modeled tools. With solid modeled tools you can set the parameters in the model parameters for the speeds and feed if you want.
What are the benifit's of solid modeled tools? This is getting complicated . Also Steve you are saying you just manually change the tool position when you program? That's what we do now and am wondering if that was the best route that's why I am working on creating a library. Solid tool models sounds intriguing.
Pro man does not gouge check the shank of its tools well. If you run a necked down 1/8 ball with 1/4 shank it is nice to have a solid model of the tool to help avoid collisions.
Can't view here at work, restricted. Will have to look at home later. I think I got that figured out though. Made a new machine with the tools in it. Also found that the PPRINT is what i needed to get the tools, date ect in the program when it is posted out. Any info on this Solid Tool Creation?
I have a pdf file on how to make solid tools but I can't attach it to the post. Not sure how to send me your email and I will send it
My ears were burning
Regarding setting the offset # to be the same as the tool number, that's a good job for the post processor to do. There isn't an automatic way to do it in the tool manager, as you have said. So, here is a FIL routing to insert in your post processor that will see if the tool offset is not set, and then will set it to the tool number:
DMY=POSTF(20) $$ save current CL record
DMY=POSTF(21) $$ restore saved record
$$ Add offset number if not programmed
NBEL=POSTF(5) $$ Number of word
IF (NBEL.EQ.4) THEN
$$ Only the tool number has been programmed
$$ Add ADJUST, Offset number=tool
$$ Increase number of word
$$ Process record
Unless I read it wrong, I think that is what Jeff was looking to do.
If it's a matter of extracting, for example, the "12" from the toon name T12, and using this as the number, then again that is probably something that can also be done in the post (but I'm no post expert!)
Many people will build a tool library by naming tools like EM_05000, BAL_02500, etc. rather than T6, T12, etc. They will let the tool number speak for itself, rather than the name.
I jope this all helps you, Jeff!
Very busy but well, thanks. I hope the same for you.
I knew Jeff Euclide was in good hands when I saw you and Nick replying to him!
Thats what is nice about Planet PTC We all help each other with problems. Makes life easier for us Manufacturing guys who usually are forgotten about in our dirty noisy machine shops.
All is well Jeff. Finally downloaded Creo Parametric1.0.... lots of learning to be done with that change. then Creo 2.0 in a few weeks... saw a power point presentaion on all the changes and it looks impressive.
Can you please help me in getting Post processor for HAAS VF4 (4th Axis)?
Have you tried creating site files for you generic milling parameters and building in equations in the machine parameters for speeds and feeds. For example I have A site file set up for the way I like to machine using trajectory I have for instance by spindle speed (sfm*3.82)/CUTTER_DIAM pro will do the math for you. Pro will automatically grab the tool diameter and also number of teeth and any other tool info and plug all the correct numbers in for the parameters. The only downfall is for machining different materials you have to change your sfm and chip per tooth. In the cut feed box I have the equation (SPINDLE_SPEED*CPT*NUMBER_FLUTES) also I have the step depth, plunge feed, step over setup on equations. This wording in the equations might not be exact because I do not have pro pulled up at the moment. But if you go to tools set-up and select tool info at the top A window will pop open with all the tool info words in the box's and those are the correct words to use for the equations. I will try to post A sample of my equations tomorrow. It sounds like a lot of work but it is real simple you basically will have your site files saved for you differnt toolpaths you can name them what ever you want and save as many as you want. Then when you create A toolpath you just open your site it fills in the parameters and that is it. As fas as your tool offset question goes if you always use the same tools on A particular work cell maybe you should just save A tool library to the work cell then the tool you want are always in the same pocket. I will post A sample of my parameters so you can try it out if you want.