How Much Help Should I Expect from my Reseller?

[DanR]

Today was filled with more frustrations... good thing we are not into manufacturing or we would go broke!

 

While trying to change WCS orientation of a part imported from Solidworks, I did a 180 rotation so that my path didn't crash on a protruding 1.5 inch shaft coming out of a crankshaft cam for a small steam engine. Everything looked right, and verified. When I went to the CNC and did a graphics check, it told me that I didn't have an A axis. On investigating, it looks like the program decided to solve the pathing problem by just rotating 4th and 5th axes. Problem is that I only have three axes.

 

I reflected on the generic machine post I have, and wonder if I shouldn't have one for a Haas Super Mini mill that precludes using solutions for which I don't have capability.

 

So far, I haven't even been able to get simple MasterCam answers from my reseller who hasn't refused to answer, but always refers me to his software expert who is never there... and I can't usually wait a day or two so I look for a work around.

 

Should I expect my reseller to provide a more specific post?

[gcode]

The generic mill is not a suitable post for a 3 axis mill, especially if you are still learning.

If you make an error in WCS, the post will do its best to comply.

Go here download, Mastercam X2 MR2 Machine Definitions and run it.

I'm pretty sure they have a good Haas post in there. It will yell at you if your tool planes aren't right ... instead of giving you usless code.

 

For WSC.. use the WCS to align your part, then set both Tool Plane and Construction plane to Top

Be careful where your origin is.

That should get you good three axis code.

 

An easier solution is to create a coordinate system in Solidworks that correctly aligns your model. Then export as a parasolid, selecting the coordinate system on the file export options page. (Save As-- choose X_B then the options dropdown)

When you import the resulting parasolid into Mastercam it will maintain the orientation you defined in SW.

[YoDoug®]

Rotary axis positioning moves are driven by toolplane. if you create a new WCS and use the corresponding toolplane to that WCS you will not get the axis rotation. If your toolplane does not mach your WCS it will post axis rotation within limits set by your machine def.

 

There are a few really informative WCS tutorials on the FTP site.

[Colin Gilchrist]

I think your post is setup to output the A axis value no matter what. All you really need to do is remove the "rotary A axis" component from your machine definition and this should eliminate the A axis code output. That being said, some resellers are better than others at support. You will find an incredible amount of support on this forum from other Mastercam users, typically within an hour or two.

 

When you say "I did a 180 degree rotation", are you rotating the geometry or using WCS - Rotate WCS? Two totally different things. There is a "Mastercam Reference Guide" under the Help menu. It has almost 30 pages on how to use the WCS, Tool, and Construction planes.

 

Again, I suspect your MD/CD/Post is the issue here. There is a HAAS specific post that should be available from your Reseller. This is a HAAS specific post created by CNC Software. This post might also have an A axis component and if so, you would have to remove it as well.

 

To fix this ouput, go to Settings|Machine Definition Manager

Now expand your machine tree and delete the A axis component. After deleting the A axis, you will need to modify your axis combination to include only X,Y,Z components.

 

HTH,

[DanR]

Wow! Like hitting the jackpot in Vegas! Three great responses.

 

gcode- Thanks for the pointer to the Machine Definitions & the SolidWorks export tip. I drew the same (simple) part twice in SolidWorks and both times I imported it, I got the part I wanted to work on in the XZ plane. I wondered why it didn't shift on one of the two. This could open a whole new world of effective moves from SW to MC.

 

DS - Thanks for the tip on the FTP site contents. I will run that down tonight.

 

Colin - Yes, it was a 'Rotate WCS' 180 after rotating it the wrong 90... I actually had the Davis book "MasterCam Level 1 with Solids" in front of me at the time. The resulting image looked right and verified in the Generic Milling Machine Verify, so we posted it, but the Haas didn't like it at all when I did a graphics run on screen. Thanks for the fix.

 

I actually cut the part. I had to draw it a fourth time but in MasterCam on the XY plane in order to get code I could run. With two of us with barely a year each under our belts with manual machines, we looked at each other after about six hours, grinned, and fired ourselves! (You have to keep a sense of humor). We spent little time on the CNC... most problems were with MasterCam issues getting the drawing oriented to give us useable code; much of that due to our inexperience with X2. Even though we both went through a semester of training on Mill 9.1 and understand what we WANT to do, trying to find the magic keystrokes to get us there has been a challenge. The internal help buttons in MC often tell you what to do, but NOT where to push the buttons to do it. With context sensitive menus, you could look a long time (and we did). At least SolidWorks gives you a button by button description of how to do the things you are researching in the help file. I guess it is always good to have something to hope for... like a new maintenance release where MasterCam has put some time and effort into those help files to bring them up to the SolidWorks level.

 

Thanks again, all! Dan.

[JNO]

Topic: How Much Help Should I Expect from my Reseller?

 

I don't think you are going to get any free "modified" posts from your reseller. But Gcode is correct, there are free HAAS posts that work fine on 3 axis machines. I would think your reseller would know that.

I know it sounds like I am kissing a$$, but we are lucky up in MA. I have never had a problem getting any assistance needed from my reseller.

Does your reseller do Netviewer? This allows your reseller to take control of your PC and help with MC issues. This has been a life saver for us.

[Jamie Betz from InterTech Supplies]

Dan do you mean Mastercam help doesn't tell you where the buttons are? If so when you are on some of the help screens at the top right there is a sentence "How do I get here" and when you click it will tell you how to get to that particular function they are discussing.

 

We are very lucky with our reseller here as well, we usually have answers within a few hours or sometimes less. We also have the capability for them to take over our PCs so they can help us get through a problem. I know some of the guys here have used it and say it is pretty awesome.

[Colin Gilchrist]

Dan,

 

One other tip for using the help file:

 

Every help dialog box has two tabs at the top. The "about" tab describes the general functions of the dialog box you are using. The "Field Definitions" tab describes in detail the function of each button. You need to switch over to the field definitions tab to learn what each button does.

 

HTH,

[George Simmons]

Dan,

[George Simmons]

Dan, I work for MLC Cad Systems as an Applications Engineer. You may be one of our customers, and we would be glad to help with any programming or posting issues. Is Jimmy your sales representitive?

[Thee Dragracer1951]

My reseller is also completely awesome. I'm buying another machine and I asked him if there was a post for a Meldas control with four axis. I had not only the post, but the mach def and control def in 10 min.

Those guys are on top of it!!

[DanR]

George, rest easy. MLC isn't the reseller.

 

Jamie, Colin, et al... Thanks, there is a lot more help available than there appeared to be. I had the Ruby Slippers, I just didn't know what to do with them...

 

I also turned off the A, B, and C rotations in Settings.

 

Today went well until I got to my last OP. I can't blame anyone but myself, but I would have sworn that I did a tool probe on T8 when I put it into the rack. I had a surfacing post for a single speed handle for a vise from TVI , and I cut one for a hex smaller than the Kurt we did there. It would have been perfect... the graphics mode ran beautifully... but having a tool that was 3 times the diameter and a half inch longer than the machine thought it was made for an interesting lesson. I was holding the part in soft jaws, and the part was aluminum, so I have a new 'modern' design for a single speed handle for a small vise. The back is cut down to save weight (yup, that's it, intentional to save weight).

 

Before long, I will have more commandments than Moses....

 

I. Thou shalt always run verify, on-machine graphics, and check the lowest Z value in the program before cutting to make sure you don't get surprised

II. Thou shalt always check tools immediately before use, especially since the Renishaw Probe makes it so easy.

III...

[gcode]

4. Thou shall always single block first approach moves on new programs.

5. Thou shall always watch "distance to go"

and heed its advice.

DTG is your vey best friend

[LaszloK]

You are not tied to your current reseller. If you do not like the service and can get another reseller in your area that would be an option for you.

[DanR]

gcode -

 

--------------------------------------------------------------------------------

4. Thou shall always single block first approach moves on new programs.

5. Thou shall always watch "distance to go"

and heed its advice.

DTG is your vey best friend

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

 

Good ones. I didn't catch the fact that the larger tool radius had me somewhat 'inside' my path, but also somewhat outside. The machine didn't know my tool was .4 inches longer and three times the diameter of that shown in the tool offset. It took me a while to figure out what happened since everything seemed right but the cut.

 

I learned to take new programs down to .5, and .1 and always single block and option stop at 5% rapids on a new program. When I was at .5 I thought I was at .1 and the difference of .4 on the tool length created a mindset where I saw .1 to go and thought it was dead on. Attention to detail required...

 

Usually, the instructor said, if everything is right at .1 above, you can take the single block off and go... I would think that tool depth and diameter problems are the ones that could get you the most.

 

I should have seen the initial cut cutting deeper than the machine code told me, but when that coolant starts to hit the tool, you can hardly see anything. Somebody suggested RainX, but I don't know how long it will hold up being pelted by the Blaser coolant.

 

The 'rest of the story' is that I took my unintentionally redesigned vise handle out of the soft jaws and finished it today. Everybody liked it better than the standard one... and it is lighter weight as well. I guess anybody can do it right, but there is something to be said about being able to recover (and learn) from your mistakes. Fortunately it wasn't something that had to be done to a particular specification.

 

Thanks.

[Thee Dragracer1951]

Are you using wear comp?????

That way you use zero's in the geometry page of your control. One less thing to have to remember to change.

There are other advantages as well. Also...standard tooling in your machine will reduce the occurance of length offset errors.

They will already be set.

[DanR]

I have been told I have to use 'control comp' since I have Rennishaw Probes. Is this correct?

[iowajim62]

quote:

---

I have been told I have to use 'control comp' since I have Rennishaw Probes. Is this correct?

---

No, the probe doesn't have anything to do with cutter compensation.

[DanR]

Maybe I should have said "Comp Type"...

 

Anyway, I think I finally got it straight, Thanks.

[iowajim62]

Dan,

I was reading the other thread and the resulting confusion I believe on my part was thinking you were using a spindle probe. Not thinking about the TSR27 setting your tools length and diameter. We only set the length of tools and check for broken tools with ours. I program with another software than Mcam but still use the same method of wear type to get G41Dxx in the program and be able to use cutter comp to adjust. Glad you got it figured out.