Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Problems with custom tool file or data?


gargodude
 Share

Recommended Posts

I am trying to create a custom tool profile for a small single-point thread mill. I've managed to do this several times in the past, but when I select the file with the profile, I get a warning message that says "Problems with custom tool file or data". I've checked the chain for gaps and different Z levels and all the usual stuff, but Mastercam (X3) won't let me use it. I've even tried it with and without the centerline. Makes no difference. Any ideas here? File is attached.

THREADMILL SCT SPTM-098L .MCX

Link to comment
Share on other sites

I am trying to create a custom tool profile for a small single-point thread mill. I've managed to do this several times in the past, but when I select the file with the profile, I get a warning message that says "Problems with custom tool file or data". I've checked the chain for gaps and different Z levels and all the usual stuff, but Mastercam (X3) won't let me use it. I've even tried it with and without the centerline. Makes no difference. Any ideas here? File is attached.

 

You've got two bogus lines off to the right of the tool. Delete them and you'll be good to go.

Link to comment
Share on other sites

You've got two bogus lines off to the right of the tool. Delete them and you'll be good to go.

Thank you very much. Works great now. Couldn't see the little xxxx at first until I changed the color, then they stuck out like a sore thumb. Sometimes it takes a younger pair of eyes. :)

Link to comment
Share on other sites
  • 7 months later...

a quick check sometimes on the "screen statistics" for custom tool profiles will tell you the number of lines, arcs, etc... on your screen. Sometimes that helps.

 

I am trying the same thing in X5 with a custom tool file for a step drill. Cant get that to work either. I am getting the same message.

Link to comment
Share on other sites

I am trying the same thing in X5 with a custom tool file for a step drill. Cant get that to work either. I am getting the same message.

 

Okay... I finally got this to work. How? I dont know. First off I had the step drill drawn up like it was a lathe part. Only half of it. Then I mirrored the geometry about 2 points to get the full tool. I then joined the two lines that made up the end of the opposite the drill point. I then added a center line. Saved the file. Then I removed the centerline and deleted half of the tool again. Now the message has gone away and the tool displays in the backplot properly. I did use "Undefined" as well from the outset of all of this. Why is this such as hassle?

Link to comment
Share on other sites

you got it to work and it sounds correct. You don't or shouldn't have to draw the whole diameter of the tool, only half of it. Sometimes it just takes redoing it the same way and it will work. I dunno. It does become easier the more you do it, though. Glad you got it.

 

Thanks for the reply.

It is correct because I ran the verifier on the tool path, then compared that back to an .stl file of the part.

I just wish I knew what I did to get it to work. I was told by a co-worker months ago that all you had to do is create an undefined tool and draw your tool geometry to scale and it should work.

I thought I had it figured out months ago but when I went to try it again yesterday it wouldnt work.

I am working in X5 but will be upgrading to X6 in a couple of months.

Link to comment
Share on other sites
  • 6 years later...

I just posted this on another thread but for someone who searches this and comes across this thread instead of the other one I'll post it here too. I would make a link to the other thread however I think these links get broken over time.

Ok I figured this out. After 3 hours using every possible combination of geometry configuration.

 The idea is to create a custom tool using the only the Tool Manager Program and a DXF file. I have attached the Mastercam File which I used to create the DXF for eveyone's reference.

 The DXF MUST have the following attributes.

 1 – 2 levels must be created and named as CUT and NOCUT

2- The geometry must be created on the upper left hand quadrant on the default TOP plane and on the CUT level

3- The length of the tool will be along the X axis (X-) and the diameter of the tool must be along the Y-axis (Y+)

4 – The tip of the tool must be placed at the origin

5 – The profile of the tool must be closed by a center line (ie. axis of rotation at Y Zero)

Save the file as a DXF  and load the DXF file and voila! There is a reason to doing it from the Tool Manager and not the Mastercam Interface which would take a while to explain. If anyone wants me to explain it let me know.

 My question is….where in any documentation does Mastercam tell me that this is required?? I have searched endlessly and could not find the prerequisites to what is required for the DXF file. 

DRILL.mcam

Link to comment
Share on other sites

Ok...I'm hesitating to post the reason due to my lack of knowledge in Mastercam, but here it goes...I could be wrong about this...but the real reason to create the tool in the Tool Manager program is because of the holder not the tool. However creating the holder in the Tool Manager Program follows the same process as creating the tool other than the fact that you place the holder on the NOCUT layer.

 I BELIEVE (based on limited experience) When you create a holder within the Mastercam interface the only way to get that holder into your library is to marry it up with a tool upon the creation of a toolpath and then export or "save" that "tool assembly" into the library by selecting the tool within the tool manager and right clicking the tool and selecting "Save to Library".

Here is the issue with this....when you open that tool library in the Tool Manager program you will find the tool assembled with the holder in tool "Assemblies" I cant figure out a way to get the Holder into the "Holders Section" So that I can use the holder on different tools. Basically the holder is locked to that tool. 

By creating the holder within the Tool Manager Program I define it as a holder. That holder can now be "Assembled" with various tools.

Someone can correct me if I'm missing something.

Link to comment
Share on other sites

It can be done, I personally manage my holders and tools in separate tool dbs just for this.  Then, I join them into machine specific dbs.  It seems to be a little smoother to use holders and tools when maintained separately.  Keep in mind I've only been using Mastercam for 5 years and am biased by existing perception of how it "should" work coming from 11 years of other softwares.

Link to comment
Share on other sites
27 minutes ago, jlw™ said:

It can be done, I personally manage my holders and tools in separate tool dbs just for this.  Then, I join them into machine specific dbs.  It seems to be a little smoother to use holders and tools when maintained separately.  Keep in mind I've only been using Mastercam for 5 years and am biased by existing perception of how it "should" work coming from 11 years of other softwares.

This is a good idea to some extent. How did you build your holders? Did you build them within the Tool Manager Program or did you build them within Mastercam and then export them somehow to your ToolDatabase. "Somehow" is the key word. I don't know how to build a holder within Mastercam and save just the holder to a tool database that when opened with the Tool Manager Program it recognizes it as a Tool Holder. The only way I know how to do this is just to build the holder within the Tool Manager Program by importing a DXF file or by using the tool holder builder.

The reasoning behind this is that I'm trying to standardize projection lengths so that operators  and programmers don't use random projection lengths when building tools. If your using a 3/8 Endmill with a 1.00" flute length then the standard projection length would be either 1.500" or 1.375". It's all about automation. Automation works better when things are standardized. 

Link to comment
Share on other sites

I build them in both.  If I only need to build one, I usually do it on the fly inside of Mastercam.  If I have for example bought a new batch of holders or have a new customer I will use the Tool Manager to create them - it flows better when creating multiple tools.

I'm on a new laptop and haven't installed Screencastomatic yet but if no one has beat me to it I'll make a video later today.

You can edit projection much easier now.  You can also use the "check holder" function as well as edit the tool on the fly by clicking and dragging projection.

So far, the only question I see that you have is how to create a holder (just a holder) in a tool db inside of Mastercam, correct?  What verion?

Link to comment
Share on other sites

Hi Jlw. Thanks for your feedback. You are correct, the only question I have is how to export just the holder which I have created in Mastercam to a Tool Database so that it can be assembled with other tools within the Tool Manager Program. I am running Mastercam Version  2019. If you have that answer I would like to know and I appreciate your efforts on this. It's no biggie however because I now know the prerequisites for the DXF file so I can do it within the Tool Manager Program

 

Link to comment
Share on other sites
5 hours ago, M4573RMZD said:

Hi Jlw. Thanks for your feedback. You are correct, the only question I have is how to export just the holder which I have created in Mastercam to a Tool Database so that it can be assembled with other tools within the Tool Manager Program. I am running Mastercam Version  2019. If you have that answer I would like to know and I appreciate your efforts on this. It's no biggie however because I now know the prerequisites for the DXF file so I can do it within the Tool Manager Program

 

Quick little video here of how to create and save a holder inside of Mastercam.  You can even create new tool databases and save them.

 

 

  • Like 1
Link to comment
Share on other sites
  • 2 weeks later...
On 2/19/2019 at 9:00 PM, jlw™ said:

Quick little video here of how to create and save a holder inside of Mastercam.  You can even create new tool databases and save them.

Thank-you jlw! That's exactly what I was missing. I didn't realize there was a contextual menu at the holder section which allowed the creation and saving of Tool Holders as well as libraries. Thats pretty decent of you. Thanks for your efforts. Perfect.

  • Like 1
Link to comment
Share on other sites
  • 1 year later...

I am Trying to create a custom tool , it’s a double angle chamfer tool and I keep getting this message . Problem with custom geometry file or data . Check for gaps , overlaps , or blanked / hidden entities . I’ve done everything it says and I just can’t get it to work . Any advise helps . Thanks .

Link to comment
Share on other sites
  • 5 months later...

Hey guys, has anyone else come across this?  No matter what I do, if there is a radius at the end of the holder, I get a concave cone on the end of the holder.  This causes tools to not assemble in Tool Manager.  Chamfers on the end of holders are not a problem.  This is what my .dxf looks like.  Level 1 is "CUT" with 0 entities, level 2 is "NOCUT" with all of the entities.

image.png.372b3cea20b52f6615957a23ab406d87.png

image.thumb.png.a4332878e6f4aa64686906cc1ba627ff.png

Link to comment
Share on other sites

try taking out the center line 

if I use a center line on my dxf files to import my custom tools into the tool manager, it will not work

it creates a flat bottom on my tools without the center line

 

and my level one is "CUT" with all my entities and level 2 is "NOCUT" with no entities

  • Like 1
Link to comment
Share on other sites
  • 1 year later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...